CFX-Pre User`s Guide

CFX-Pre User`s Guide
ANSYS CFX-Pre User's Guide
ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
[email protected]
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
Release 14.0
November 2011
ANSYS, Inc. is
certified to ISO
9001:2008.
Copyright and Trademark Information
© 2011 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.
ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any
and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or
trademarks of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used
by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service
and feature names or trademarks are the property of their respective owners.
Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products
and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement
that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting
laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products
and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions
of that software license agreement.
ANSYS, Inc. is certified to ISO 9001:2008.
U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use,
duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc.
software license agreement and FAR 12.212 (for non-DOD licenses).
Third-Party Software
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software
and third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.
Published in the U.S.A.
Table of Contents
1. CFX-Pre Basics ......................................................................................................................................... 1
1.1. Starting CFX-Pre ............................................................................................................................... 1
1.2. CFX-Pre Modes of Operation ............................................................................................................. 2
1.3. Working with the CFX-Pre Interface ................................................................................................... 3
1.3.1. Viewer ..................................................................................................................................... 4
1.3.2. CFX-Pre Workspace .................................................................................................................. 4
1.3.2.1. Outline Tree View ............................................................................................................ 5
1.3.2.1.1. General Considerations ........................................................................................... 5
1.3.2.1.2. Outline Tree View Structure ..................................................................................... 5
1.3.2.1.2.1. Outline Tree View Shortcut Menu Commands ................................................. 7
1.3.2.2. Details View .................................................................................................................... 9
1.3.3. Physics Message Window ....................................................................................................... 11
1.3.3.1. Physics Errors from Old .def/.res Files .............................................................................. 12
1.3.3.2. Physics Message Window Shortcut Menu Commands ..................................................... 12
1.3.4. Menu Bar ............................................................................................................................... 13
1.3.5. Toolbar .................................................................................................................................. 13
1.4. CFX-Pre File Types ........................................................................................................................... 13
2. CFX-Pre 3D Viewer ................................................................................................................................ 17
2.1. Object Visibility ............................................................................................................................... 18
2.2. 3D Viewer Modes and Commands ................................................................................................... 19
2.2.1. 3D Viewer Toolbar .................................................................................................................. 19
2.2.2. Shortcut Menus ..................................................................................................................... 21
2.2.2.1. CFX-Pre 3D Viewer Shortcut Menu ................................................................................. 22
2.2.2.1.1. Shortcuts for CFX-Pre (Viewer Background) ........................................................... 22
2.2.2.1.2. Shortcuts for CFX-Pre (Viewer Object) ................................................................... 23
2.2.3. Viewer Hotkeys ...................................................................................................................... 23
2.2.4. Mouse Button Mapping .......................................................................................................... 24
2.2.5. Picking Mode ......................................................................................................................... 26
2.2.5.1. Selecting Objects .......................................................................................................... 26
2.2.6. Boundary Markers and Labels ................................................................................................. 27
2.2.6.1. Label Options ................................................................................................................ 27
2.2.6.2. Boundary Markers ......................................................................................................... 27
2.2.6.3. Boundary Vectors .......................................................................................................... 27
2.3. Views and Figures ........................................................................................................................... 27
2.3.1. Switching to a View or Figure .................................................................................................. 28
2.3.2. Changing the Definition of a View or Figure ............................................................................ 28
2.4. Stereo Viewer ................................................................................................................................. 28
3. CFX-Pre File Menu ................................................................................................................................. 31
3.1. New Case Command ....................................................................................................................... 31
3.2. Open Case Command ..................................................................................................................... 32
3.2.1. Recover Original Session ........................................................................................................ 32
3.2.2. Opening Case (.cfx) Files ......................................................................................................... 33
3.2.3. Opening CFX-Solver Input (.def, .mdef ), Results (.res), Transient (.trn) or Backup (.bak) Files ....... 33
3.2.4. Opening CCL (.ccl) Files .......................................................................................................... 33
3.2.5. Opening Meshing (.cmdb or .dsdb) Files ................................................................................. 33
3.2.6. Opening CFX-Mesh (.gtm) Files ............................................................................................... 34
3.3. Close Command ............................................................................................................................. 34
3.4. Save Case Command ....................................................................................................................... 34
3.5. Save Project Command ................................................................................................................... 34
3.6. Refresh Command (ANSYS Workbench only) ................................................................................... 34
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
iii
ANSYS CFX-Pre User's Guide
3.7. Save Case As Command .................................................................................................................. 34
3.8. Import Mesh Command .................................................................................................................. 34
3.9. Reload Mesh Files Command .......................................................................................................... 34
3.10. Import CCL Command .................................................................................................................. 35
3.10.1. Append or Replace ............................................................................................................... 35
3.10.1.1. Append ....................................................................................................................... 35
3.10.1.2. Replace ....................................................................................................................... 36
3.10.1.2.1. Auto-load materials ............................................................................................. 36
3.11. Export CCL Command ................................................................................................................... 36
3.11.1. Save All Objects .................................................................................................................... 36
3.11.1.1. Sample of Saving CEL Expressions ................................................................................ 36
3.12. Save Picture Command ................................................................................................................. 37
3.13. Recent Case Files Submenu ........................................................................................................... 38
3.14. Recent CCL Files Submenu ............................................................................................................ 38
3.15. Recent Session Files Submenu ....................................................................................................... 38
3.16. Quit Command ............................................................................................................................. 39
4. CFX-Pre Edit Menu ................................................................................................................................ 41
4.1. Undo and Redo ............................................................................................................................... 41
4.2. Options .......................................................................................................................................... 42
4.2.1. CFX-Pre Options ..................................................................................................................... 42
4.2.1.1. General ......................................................................................................................... 43
4.2.1.1.1. Auto Generation ................................................................................................... 43
4.2.1.1.2. Physics ................................................................................................................. 44
4.2.1.2. Graphics Style ............................................................................................................... 44
4.2.1.2.1. Object Highlighting .............................................................................................. 44
4.2.1.2.2. Background .......................................................................................................... 45
4.2.1.2.2.1. Color ............................................................................................................ 45
4.2.1.2.2.2. Image .......................................................................................................... 45
4.2.1.2.3. Colors ................................................................................................................... 45
4.2.1.2.3.1. Labels .......................................................................................................... 45
4.2.1.2.3.2. Legend Text and Turbo Axis .......................................................................... 45
4.2.1.2.4. Visibility ................................................................................................................ 46
4.2.1.2.4.1. Axis and Ruler Visibility ................................................................................. 46
4.2.1.3. Render .......................................................................................................................... 46
4.2.1.4. Mesh ............................................................................................................................. 46
4.2.1.4.1. Mesh Import Options ............................................................................................ 46
4.2.1.5. Turbo ............................................................................................................................ 46
4.2.1.6. Labels and Markers ........................................................................................................ 46
4.2.1.6.1. Labels ................................................................................................................... 46
4.2.1.6.2. Boundary Markers ................................................................................................. 46
4.2.1.6.3. Boundary Vectors .................................................................................................. 47
4.2.1.7. Extensions ..................................................................................................................... 47
4.2.1.8. Customization ............................................................................................................... 47
4.2.1.9. Solve ............................................................................................................................. 47
4.2.1.10. Viewer ......................................................................................................................... 47
4.2.2. Common Options ................................................................................................................... 47
4.2.2.1. Appearance ................................................................................................................... 48
4.2.2.2. Viewer Setup ................................................................................................................. 48
4.2.2.2.1. Double Buffering .................................................................................................. 48
4.2.2.2.2. Unlimited Zoom .................................................................................................... 48
4.2.2.3. Mouse Mapping ............................................................................................................ 48
4.2.2.4. Units ............................................................................................................................. 48
iv
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
4.2.2.4.1. Additional Help on Units ....................................................................................... 49
5. CFX-Pre Session Menu ........................................................................................................................... 51
5.1. New Session Command .................................................................................................................. 51
5.2. Start Recording and Stop Recording Commands ............................................................................. 52
5.3. Play Session and Play Tutorial Commands ........................................................................................ 52
5.3.1. Play Session Command .......................................................................................................... 52
5.3.2. Play Tutorial Command .......................................................................................................... 53
6. CFX-Pre Insert Menu ............................................................................................................................. 55
7. CFX-Pre Tools Menu .............................................................................................................................. 59
7.1. Command Editor ............................................................................................................................ 59
7.2. Expand Profile Data ......................................................................................................................... 59
7.3. Initialize Profile Data ....................................................................................................................... 60
7.4. Macro Calculator ............................................................................................................................. 60
7.5. Solve .............................................................................................................................................. 60
7.5.1. Write Solver Input File Command ............................................................................................ 61
7.6. Applications ................................................................................................................................... 61
7.7. Quick Setup Mode .......................................................................................................................... 61
7.8. Turbo Mode .................................................................................................................................... 61
8. CFX-Pre Extensions Menu ..................................................................................................................... 63
9. Importing and Transforming Meshes ................................................................................................... 65
9.1. Importing Meshes ........................................................................................................................... 65
9.1.1. Importing Multiple Meshes .................................................................................................... 65
9.1.2. Common Import Options ....................................................................................................... 66
9.1.2.1. Mesh Units .................................................................................................................... 66
9.1.2.2. Assembly Prefix ............................................................................................................. 66
9.1.2.3. Primitive Strategy .......................................................................................................... 66
9.1.2.4. Ignore Invalid Degenerate Elements ............................................................................... 66
9.1.2.5. Duplicate Node Checking .............................................................................................. 67
9.1.3. Supported Mesh File Types ..................................................................................................... 67
9.1.3.1. ANSYS Meshing Files ..................................................................................................... 67
9.1.3.1.1. Named Selections ................................................................................................. 68
9.1.3.1.2. Contact Detection Settings ................................................................................... 68
9.1.3.2. CFX-Mesh Files .............................................................................................................. 69
9.1.3.3. CFX-Solver Input files ..................................................................................................... 69
9.1.3.4. ICEM CFD Files ............................................................................................................... 69
9.1.3.5. ANSYS Files ................................................................................................................... 69
9.1.3.6. FLUENT Files .................................................................................................................. 70
9.1.3.6.1. Override Default 2D Mesh Settings ........................................................................ 70
9.1.3.6.1.1. Interpret 2D Mesh as .................................................................................... 70
9.1.3.6.1.1.1. Axisymmetric ...................................................................................... 70
9.1.3.6.1.1.2. Planar .................................................................................................. 70
9.1.3.7. CGNS Files ..................................................................................................................... 70
9.1.3.7.1. Importing CGNS files into CFX ............................................................................... 71
9.1.3.7.1.1. Method ........................................................................................................ 71
9.1.3.7.1.2. Base (Base_t) ................................................................................................ 71
9.1.3.7.1.3. Zone (Zone_t) .............................................................................................. 71
9.1.3.7.1.4. Elements (ElementSection_t) ........................................................................ 71
9.1.3.7.1.5. Element Types Supported ............................................................................. 71
9.1.3.7.1.6. Boundary Conditions (BC_t) ......................................................................... 71
9.1.3.7.1.7. Families (Family_t, FamilyBC_t, FamilyName_t) .............................................. 72
9.1.3.7.1.8. Grid Connectivity (GridConnectivity_t and GridConnectivity1to1_t) .............. 72
9.1.3.7.1.9. CGNS Data Ignored ...................................................................................... 72
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
v
ANSYS CFX-Pre User's Guide
9.1.3.7.2. Prefix regions with zone name .............................................................................. 72
9.1.3.7.3. Create Regions From: Element Sections ................................................................. 73
9.1.3.7.4. Create Regions From: Boundary Conditions ........................................................... 73
9.1.3.7.5. Create Regions From: Families ............................................................................... 73
9.1.3.7.6. Create Regions From: Connectivity Mappings ........................................................ 73
9.1.3.7.7. Example of Create Regions From ........................................................................... 73
9.1.3.7.8. Read Only One CGNS Base .................................................................................... 73
9.1.3.8. CFX-TASCflow Files ........................................................................................................ 74
9.1.3.8.1. Convert 3D Region Labels to Regions .................................................................... 74
9.1.3.8.2. Grid Connections Processed (in the .grd file) .......................................................... 74
9.1.3.8.3. Grid Embedding ................................................................................................... 75
9.1.3.8.4. Retain Block-off .................................................................................................... 75
9.1.3.8.5. Regions in the .grd file .......................................................................................... 75
9.1.3.8.6. Boundary Conditions in .bcf File ............................................................................ 76
9.1.3.8.7. Regions in the .gci File ........................................................................................... 76
9.1.3.8.8. Importing CFX-TASCflow TurboPre MFR Grids ........................................................ 76
9.1.3.8.9. Parameter File ....................................................................................................... 76
9.1.3.9. CFX-4 Grid Files ............................................................................................................. 76
9.1.3.9.1. Split Symmetry Planes ........................................................................................... 77
9.1.3.9.2. Import from Cylindrical Coordinates ...................................................................... 77
9.1.3.9.3. Create 2D Regions on ............................................................................................ 77
9.1.3.9.4. Create 3D Regions on ............................................................................................ 77
9.1.3.9.5. Blocked Off Regions (SOLIDs) ................................................................................ 78
9.1.3.9.6. Conducting Solid Regions (SOLCONs) .................................................................... 78
9.1.3.9.7. Import 2D Axisymmetric Mesh .............................................................................. 78
9.1.3.9.8. Importing MFR Grids ............................................................................................. 78
9.1.3.10. CFX-BladeGenPlus Files ................................................................................................ 79
9.1.3.11. PATRAN Neutral Files .................................................................................................... 79
9.1.3.12. IDEAS Universal Files .................................................................................................... 79
9.1.3.13. GridPro/az3000 Grid Files ............................................................................................. 79
9.1.3.14. NASTRAN Files ............................................................................................................. 80
9.1.3.15. Pointwise Gridgen Files ................................................................................................ 80
9.1.3.16. User Import ................................................................................................................. 80
9.2. Mesh Tree View ............................................................................................................................... 81
9.2.1. Shortcut Menu Commands for Meshes and Regions ................................................................ 81
9.3. Deleting Meshes and Mesh Components from the Tree View ........................................................... 81
9.4. Transform Mesh Command ............................................................................................................. 82
9.4.1. Target Location ...................................................................................................................... 82
9.4.2. Reference Coord Frame .......................................................................................................... 83
9.4.3. Transformation: Rotation ........................................................................................................ 83
9.4.3.1. Rotation Option: Principal Axis ....................................................................................... 83
9.4.3.2. Rotation Option: Rotation Axis ....................................................................................... 83
9.4.3.3. Rotation Angle Option ................................................................................................... 83
9.4.3.3.1. Specified .............................................................................................................. 83
9.4.3.3.2. Full Circle .............................................................................................................. 83
9.4.3.3.3. Two Points ............................................................................................................ 83
9.4.4. Transformation: Translation ..................................................................................................... 84
9.4.4.1. Method: Deltas .............................................................................................................. 84
9.4.4.2. Method: Vectors ............................................................................................................. 84
9.4.5. Transformation: Scale ............................................................................................................. 84
9.4.5.1. Method: Uniform ........................................................................................................... 84
9.4.5.2. Method: Non Uniform .................................................................................................... 84
vi
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
9.4.5.3. Scale Origin ................................................................................................................... 84
9.4.5.4. Apply Scale To ............................................................................................................... 85
9.4.6. Transformation: Reflection ...................................................................................................... 85
9.4.6.1. Method ......................................................................................................................... 85
9.4.6.2. Apply Reflection To ........................................................................................................ 85
9.4.7. Transformation: Turbo Rotation ............................................................................................... 86
9.4.7.1. Rotation Option: Principal Axis ....................................................................................... 86
9.4.7.2. Rotation Option: Rotation Axis ....................................................................................... 86
9.4.7.3. Rotation Axis Options .................................................................................................... 86
9.4.8. Multiple Copies ...................................................................................................................... 86
9.4.8.1. # of Copies .................................................................................................................... 86
9.4.8.2. Delete Original .............................................................................................................. 87
9.4.9. Advanced Options ................................................................................................................. 87
9.4.9.1. Glue Adjacent Meshes ................................................................................................... 87
9.4.10. Automatic Transformation Preview ....................................................................................... 88
9.5. Gluing Meshes Together ................................................................................................................. 88
9.6. Mesh Editor .................................................................................................................................... 88
9.7. Render Options .............................................................................................................................. 88
9.7.1. Render Options Dialog Box ..................................................................................................... 89
9.7.1.1. Draw Faces .................................................................................................................... 89
9.7.1.2. Face Color ..................................................................................................................... 89
9.7.1.3. Transparency ................................................................................................................. 89
9.7.1.4. Draw Mode/Surface Drawing ......................................................................................... 89
9.7.1.4.1. Flat Shading .......................................................................................................... 89
9.7.1.4.2. Smooth Shading ................................................................................................... 89
9.7.1.5. Face Culling ................................................................................................................... 89
9.7.1.5.1. Front Faces ........................................................................................................... 90
9.7.1.5.2. Back Faces ............................................................................................................ 90
9.7.1.5.3. No Culling ............................................................................................................. 90
9.7.1.6. Lighting ........................................................................................................................ 90
9.7.1.7. Specular ........................................................................................................................ 90
9.7.1.8. Draw Lines .................................................................................................................... 90
9.7.1.9. Edge Angle/Render Edge Angle ..................................................................................... 90
9.7.1.10. Line Width ................................................................................................................... 90
9.7.1.11. Line Color .................................................................................................................... 90
9.7.1.12. Visibility ...................................................................................................................... 90
9.7.2. Render Options - Multiple 2D Regions .................................................................................... 90
9.8. Mesh Topology in CFX-Pre ............................................................................................................... 91
9.8.1. Assemblies, Primitive Regions, and Composite Regions ........................................................... 91
9.8.1.1. Composite Regions ........................................................................................................ 92
9.8.1.1.1. Applications of the Composite Regions ................................................................. 92
9.8.2. Domain and Subdomain Locations ......................................................................................... 92
9.8.3. Boundary Condition and Domain Interface Locations .............................................................. 93
9.8.4. Importing Multi-domain Cases ............................................................................................... 93
9.9. Advanced Topic: cfx5gtmconv Application ....................................................................................... 93
10. Regions ................................................................................................................................................ 95
10.1. Primitive Regions .......................................................................................................................... 95
10.2. Composite Regions ....................................................................................................................... 95
10.3. Using Regions in CFX-Pre .............................................................................................................. 96
10.4. Editing Regions in CFX-Pre ............................................................................................................ 96
10.4.1. Defining and Editing Primitive Regions ................................................................................. 96
10.4.1.1. Advanced Options ....................................................................................................... 98
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
vii
ANSYS CFX-Pre User's Guide
10.4.2. Defining and Editing Composite Regions .............................................................................. 98
10.4.2.1. Union .......................................................................................................................... 99
10.4.2.2. Alias ............................................................................................................................ 99
10.5. Applications of Composite Regions ............................................................................................... 99
11. Analysis Type ..................................................................................................................................... 101
11.1. Basic Settings Tab ........................................................................................................................ 101
11.1.1. External Solver Coupling Settings ....................................................................................... 101
11.1.2. Analysis Type Settings ........................................................................................................ 101
11.1.2.1. Steady State .............................................................................................................. 102
11.1.2.2. Transient ................................................................................................................... 102
11.1.2.2.1. Time Duration ................................................................................................... 102
11.1.2.2.2. Time Steps ........................................................................................................ 102
11.1.2.2.3. Initial Time ........................................................................................................ 103
11.1.2.3. Transient Blade Row ................................................................................................... 103
12. Domains ............................................................................................................................................ 105
12.1. Creating New Domains ............................................................................................................... 105
12.2. The Details View for Domain Objects ........................................................................................... 106
12.3. Using Multiple Domains .............................................................................................................. 106
12.3.1. Multiple Fluid Domains ....................................................................................................... 106
12.3.2. Multiple Solid Domains ...................................................................................................... 107
12.4. User Interface ............................................................................................................................. 107
12.4.1. Basic Settings Tab ............................................................................................................... 107
12.4.1.1. Location and Type ...................................................................................................... 107
12.4.1.1.1. Location ............................................................................................................ 107
12.4.1.1.2. Domain Type ..................................................................................................... 107
12.4.1.1.3. Coordinate Frame ............................................................................................. 108
12.4.1.2. Fluid and Particle Definitions and Solid Definitions ..................................................... 108
12.4.1.2.1. Morphology ...................................................................................................... 109
12.4.1.2.1.1. Mean Diameter ........................................................................................ 109
12.4.1.2.1.2. Minimum Volume Fraction ........................................................................ 109
12.4.1.2.1.3. Maximum Packing .................................................................................... 109
12.4.1.2.1.4. Restitution Coefficient .............................................................................. 109
12.4.1.2.1.5. Particle Diameter Distribution ................................................................... 110
12.4.1.2.1.6. Particle Shape Factors ............................................................................... 110
12.4.1.2.1.7. Particle Diameter Change ......................................................................... 110
12.4.1.2.1.7.1. Swelling Model ................................................................................ 110
12.4.1.3. Particle Tracking ........................................................................................................ 110
12.4.1.4. Domain Models ......................................................................................................... 110
12.4.1.4.1. Pressure: Reference Pressure .............................................................................. 110
12.4.1.4.2. Buoyancy: Option .............................................................................................. 110
12.4.1.4.3. Domain Motion ................................................................................................. 111
12.4.1.4.4. Mesh Deformation ............................................................................................ 113
12.4.1.4.5. Passage Definition ............................................................................................. 113
12.4.2. Fluid Models Tab ................................................................................................................ 113
12.4.2.1. Multiphase Options ................................................................................................... 114
12.4.2.1.1. Homogeneous Model ....................................................................................... 114
12.4.2.1.2. Free Surface Model ........................................................................................... 114
12.4.2.1.3. Multiphase Reactions ........................................................................................ 114
12.4.2.2. Heat Transfer ............................................................................................................. 114
12.4.2.2.1. Homogeneous Model ....................................................................................... 114
12.4.2.2.2. Heat Transfer: Option ......................................................................................... 114
12.4.2.3. Turbulence ................................................................................................................ 115
viii
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
12.4.2.3.1. Homogeneous Model ....................................................................................... 115
12.4.2.3.2. Turbulence: Option ............................................................................................ 115
12.4.2.3.3. Buoyancy Turbulence ........................................................................................ 116
12.4.2.3.4. Wall Function .................................................................................................... 116
12.4.2.3.5. Turbulent Flux Closure for Heat Transfer ............................................................. 116
12.4.2.4. Reaction or Combustion Model .................................................................................. 116
12.4.2.4.1. Soot Model ....................................................................................................... 117
12.4.2.5. Thermal Radiation Model ........................................................................................... 117
12.4.2.6. Electromagnetic Model .............................................................................................. 118
12.4.2.7. Component Details .................................................................................................... 118
12.4.2.8. Additional Variable Details ......................................................................................... 119
12.4.3. Polydispersed Fluid Tab ...................................................................................................... 119
12.4.4. Fluid Specific Models Tab .................................................................................................... 119
12.4.4.1. Fluid List Box ............................................................................................................. 120
12.4.4.2. Kinetic Theory ............................................................................................................ 120
12.4.4.3. Heat Transfer ............................................................................................................. 120
12.4.4.3.1. Heat Transfer Option: Particle Temperature ........................................................ 121
12.4.4.4. Turbulence Model ...................................................................................................... 121
12.4.4.5. Turbulent Wall Functions ............................................................................................ 121
12.4.4.6. Combustion Model .................................................................................................... 121
12.4.4.7. Erosion Model ........................................................................................................... 121
12.4.4.8. Fluid Buoyancy Model ................................................................................................ 121
12.4.4.9. Solid Pressure Model .................................................................................................. 121
12.4.4.10. Component Details .................................................................................................. 122
12.4.4.11. Additional Variable Models ....................................................................................... 122
12.4.5. Fluid Pair Models Tab .......................................................................................................... 122
12.4.5.1. Fluid Pair List box ....................................................................................................... 122
12.4.5.2. Particle Coupling ....................................................................................................... 122
12.4.5.3. Surface Tension Coefficient ........................................................................................ 122
12.4.5.4. Surface Tension Force Model ...................................................................................... 123
12.4.5.5. Interphase Transfer Model .......................................................................................... 123
12.4.5.5.1. Particle Model ................................................................................................... 123
12.4.5.5.2. Mixture Model .................................................................................................. 123
12.4.5.5.3. Free Surface Model ........................................................................................... 123
12.4.5.5.4. None ................................................................................................................ 123
12.4.5.6. Momentum Transfer .................................................................................................. 123
12.4.5.6.1. Drag Force ........................................................................................................ 124
12.4.5.6.2. Particle User Source ........................................................................................... 124
12.4.5.6.3. Lift Force ........................................................................................................... 124
12.4.5.6.4. Virtual Mass Force ............................................................................................. 124
12.4.5.6.5. Wall Lubrication Force ....................................................................................... 124
12.4.5.6.6. Turbulent Dispersion Force ................................................................................ 124
12.4.5.6.7. Pressure Gradient Force ..................................................................................... 125
12.4.5.7. Turbulence Transfer .................................................................................................... 125
12.4.5.8. Heat Transfer ............................................................................................................. 125
12.4.5.9. Mass Transfer ............................................................................................................. 125
12.4.5.10. Additional Variable Pairs ........................................................................................... 125
12.4.5.11. Component Pairs ..................................................................................................... 126
12.4.5.11.1. Eulerian | Eulerian Pairs .................................................................................... 126
12.4.5.11.2. Continuous | Particle Pairs ............................................................................... 126
12.4.5.12. Particle Breakup ....................................................................................................... 127
12.4.5.13. Particle Collision ...................................................................................................... 127
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ix
ANSYS CFX-Pre User's Guide
12.4.6. Solid Models Tab ................................................................................................................ 128
12.4.6.1. Heat Transfer ............................................................................................................. 128
12.4.6.2. Thermal Radiation Model ........................................................................................... 128
12.4.6.3. Electromagnetic Model .............................................................................................. 128
12.4.6.4. Additional Variables Models ....................................................................................... 128
12.4.6.5. Solid Motion .............................................................................................................. 128
12.4.7. Porosity Settings Tab .......................................................................................................... 129
12.4.7.1. Area Porosity ............................................................................................................. 129
12.4.7.2. Volume Porosity ......................................................................................................... 130
12.4.7.3. Loss Models ............................................................................................................... 130
12.4.7.4. Contact Area Model ................................................................................................... 130
12.4.7.5. Fluid Solid Area Density ............................................................................................. 131
12.4.7.6. Fluid Solid Heat Transfer ............................................................................................. 131
12.4.7.7. Additional Variable Pair Details ................................................................................... 131
12.4.8. Particle Injection Regions Tab ............................................................................................. 131
12.4.8.1. Particle Injection Regions List Box .............................................................................. 131
12.4.8.2. Coordinate Frame ...................................................................................................... 131
12.4.8.3. Fluid: List Box ............................................................................................................. 132
12.4.8.4. [fluid name] Check Box .............................................................................................. 132
12.4.8.4.1. Injection Method .............................................................................................. 132
12.4.8.4.1.1. Settings for Cone Definition ...................................................................... 133
12.4.8.4.1.2. Settings for Injection Velocity .................................................................... 133
12.4.8.4.1.3. Settings for Particle Primary Breakup ......................................................... 134
12.4.9. Initialization Tab ................................................................................................................. 135
12.4.10. Solver Control Tab ............................................................................................................ 135
13. Domain Interfaces ............................................................................................................................. 137
13.1. Creating and Editing a Domain Interface ..................................................................................... 137
13.1.1. Domain Interface: Basic Settings Tab ................................................................................... 138
13.1.1.1. Interface Type ............................................................................................................ 138
13.1.1.2. Interface Side 1/2 ....................................................................................................... 138
13.1.1.2.1. Domain (Filter) .................................................................................................. 138
13.1.1.2.2. Region List ........................................................................................................ 139
13.1.1.3. Interface Models ........................................................................................................ 139
13.1.1.3.1. Interface Model Option: Translational Periodicity ................................................ 139
13.1.1.3.2. Interface Model Option: Rotational Periodicity ................................................... 139
13.1.1.3.3. Interface Model Option: General Connection ..................................................... 139
13.1.1.3.3.1. Frame Change/Mixing Model .................................................................... 139
13.1.1.3.3.1.1. Option ............................................................................................. 139
13.1.1.3.3.1.2. Frozen Rotor: Rotational Offset Check Box ........................................ 139
13.1.1.3.3.1.3. Stage: Pressure Profile Decay Check Box ........................................... 140
13.1.1.3.3.1.4. Stage: Constant Total Pressure Check Box ......................................... 140
13.1.1.3.3.2. Pitch Change Options ............................................................................... 140
13.1.1.3.3.2.1. Pitch Change: Value: Pitch Ratio ........................................................ 140
13.1.1.3.3.2.2. Pitch Change: Specified Pitch Angles: Pitch Angle Side 1/2 ................ 140
13.1.2. Domain Interface: Additional Interface Models Tab .............................................................. 140
13.1.2.1. Mass And Momentum ................................................................................................ 140
13.1.2.1.1. Conservative Interface Flux: Interface Models ..................................................... 141
13.1.2.1.1.1. None ........................................................................................................ 141
13.1.2.1.1.2. Mass Flow Rate ......................................................................................... 141
13.1.2.1.1.2.1. Pressure Update Multiplier ............................................................... 141
13.1.2.1.1.3. Pressure Change ....................................................................................... 141
13.1.2.1.2. No Slip Wall ....................................................................................................... 141
x
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
13.1.2.1.2.1. No Slip Wall: Wall Velocity .......................................................................... 141
13.1.2.1.3. Free Slip Wall ..................................................................................................... 142
13.1.2.1.4. Side Dependent ................................................................................................ 142
13.1.2.2. Heat Transfer ............................................................................................................. 142
13.1.2.2.1. Conservative Interface Flux: Interface Model ...................................................... 142
13.1.2.2.1.1. None ........................................................................................................ 142
13.1.2.2.1.2. Interface Model Option: Thermal Contact Resistance ................................. 142
13.1.2.2.1.3. Interface Model Option: Thin Material ....................................................... 142
13.1.2.2.2. Side Dependent ................................................................................................ 142
13.1.2.3. Electric Field .............................................................................................................. 142
13.1.2.3.1. Conservative Interface Flux: Interface Model ...................................................... 143
13.1.2.3.1.1. None ........................................................................................................ 143
13.1.2.3.1.2. Interface Model Option: Electric Field Contact Resistance .......................... 143
13.1.2.3.2. Side Dependent ................................................................................................ 143
13.1.2.4. Additional Variable .................................................................................................... 143
13.1.2.4.1. Conservative Interface Flux: Interface Model ...................................................... 143
13.1.2.4.1.1. None ........................................................................................................ 143
13.1.2.4.1.2. Interface Model Option: Additional Variable Contact Resistance ................. 143
13.1.2.4.2. Side Dependent ................................................................................................ 143
13.1.2.5. Conditional Connection Control ................................................................................. 143
13.1.3. Domain Interface: Solid Interface Models Tab ...................................................................... 144
13.1.3.1. Heat Transfer ............................................................................................................. 144
13.1.3.1.1. Conservative Interface Flux: Interface Model ...................................................... 144
13.1.3.1.1.1. None ........................................................................................................ 144
13.1.3.1.1.2. Interface Model Option: Thermal Contact Resistance ................................. 144
13.1.3.1.1.3. Interface Model Option: Thin Material ....................................................... 144
13.1.3.1.2. Side Dependent ................................................................................................ 144
13.1.3.2. Additional Variable .................................................................................................... 144
13.1.3.2.1. Conservative Interface Flux: Interface Model ...................................................... 145
13.1.3.2.1.1. None ........................................................................................................ 145
13.1.3.2.1.2. Interface Model Option: Additional Variable Contact Resistance ................. 145
13.1.3.2.2. Side Dependent ................................................................................................ 145
13.1.4. Domain Interface: Mesh Connection Tab ............................................................................. 145
13.1.4.1. Mesh Connection Method .......................................................................................... 145
13.1.4.1.1. Mesh Connection: Option .................................................................................. 145
13.1.4.1.2. Intersection Control .......................................................................................... 145
13.1.4.1.2.1. Intersection Control: Option ...................................................................... 146
14. Boundary Conditions ........................................................................................................................ 149
14.1. Default Boundary Condition ........................................................................................................ 149
14.2. Creating and Editing a Boundary Condition ................................................................................. 150
14.2.1. Boundary Basic Settings Tab ............................................................................................... 150
14.2.1.1. Boundary Type .......................................................................................................... 151
14.2.1.2. Location .................................................................................................................... 151
14.2.1.3. Coord Frame .............................................................................................................. 151
14.2.1.4. Frame Type ................................................................................................................ 151
14.2.1.5. Profile Boundary Conditions ....................................................................................... 151
14.2.1.5.1. Use Profile Data ................................................................................................. 152
14.2.1.5.1.1. Initializing Profile Data .............................................................................. 152
14.2.1.5.1.2. Profile Boundary Setup ............................................................................. 152
14.2.2. Boundary Details Tab .......................................................................................................... 152
14.2.2.1. Boundary Details: Inlet ............................................................................................... 153
14.2.2.1.1. Flow Regime: Inlet ............................................................................................. 153
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xi
ANSYS CFX-Pre User's Guide
14.2.2.1.2. Mesh Motion: Inlet ............................................................................................ 153
14.2.2.2. Boundary Details: Outlet ............................................................................................ 153
14.2.2.2.1. Flow Regime: Outlet .......................................................................................... 153
14.2.2.2.2. Mass and Momentum: Outlet ............................................................................. 153
14.2.2.2.3. Pressure Averaging: Outlet ................................................................................. 153
14.2.2.2.4. Thermal Radiation: Outlet .................................................................................. 153
14.2.2.2.5. Mesh Motion: Outlet .......................................................................................... 153
14.2.2.3. Boundary Details: Opening ........................................................................................ 154
14.2.2.3.1. Mass and Momentum: Opening ......................................................................... 154
14.2.2.3.2. Flow Direction: Opening .................................................................................... 154
14.2.2.3.3. Loss Coefficient: Opening .................................................................................. 154
14.2.2.3.4. Turbulence: Opening ......................................................................................... 154
14.2.2.3.5. Heat Transfer: Opening ...................................................................................... 154
14.2.2.3.6. Thermal Radiation: Opening .............................................................................. 154
14.2.2.3.7. Component Details: Opening ............................................................................ 154
14.2.2.3.8. Mesh Motion: Opening ...................................................................................... 154
14.2.2.4. Boundary Details: Wall ................................................................................................ 154
14.2.2.4.1. Mass And Momentum ....................................................................................... 154
14.2.2.4.1.1. Slip Model Settings ................................................................................... 155
14.2.2.4.1.2. Shear Stress Settings ................................................................................ 155
14.2.2.4.1.3. Wall Velocity Settings ................................................................................ 155
14.2.2.4.1.3.1. Axis Definition ................................................................................. 155
14.2.2.4.2. Wall Roughness ................................................................................................. 155
14.2.2.4.3. Solid Motion: Wall .............................................................................................. 155
14.2.2.4.4. Heat Transfer: Wall ............................................................................................. 156
14.2.2.4.5. Thermal Radiation: Wall ..................................................................................... 156
14.2.2.4.6. Mesh Motion: Wall ............................................................................................. 156
14.2.2.4.7. Additional Coupling Sent Data .......................................................................... 156
14.2.2.5. Boundary Details: Symmetry ...................................................................................... 156
14.2.2.6. Boundary Details: Interfaces ....................................................................................... 156
14.2.2.7. Mesh Motion ............................................................................................................. 156
14.2.3. Boundary Fluid Values Tab .................................................................................................. 157
14.2.3.1. Fluid Values: Turbulence ............................................................................................. 157
14.2.3.1.1. Intensity and Length Scale ................................................................................. 158
14.2.3.1.2. Intensity and Eddy Viscosity Ratio ...................................................................... 158
14.2.3.1.3. k and Epsilon .................................................................................................... 158
14.2.3.1.4. Intensity and Auto Compute Length .................................................................. 158
14.2.3.2. Fluid Values: Volume Fraction ..................................................................................... 158
14.2.3.3. Fluid Values: Heat Transfer .......................................................................................... 158
14.2.3.4. Fluid Values for Inlets and Openings ........................................................................... 158
14.2.3.4.1. Multiphase ........................................................................................................ 158
14.2.3.4.2. MUSIG settings ................................................................................................. 159
14.2.3.4.3. Particle Tracking Settings for Inlets and Openings .............................................. 159
14.2.3.4.3.1. Phase List ................................................................................................. 159
14.2.3.4.3.2. Particle Behavior ....................................................................................... 159
14.2.3.4.3.3. Mass and Momentum ............................................................................... 159
14.2.3.4.3.4. Particle Position ........................................................................................ 160
14.2.3.4.3.5. Particle Locations ..................................................................................... 160
14.2.3.4.3.6. Number of Positions ................................................................................. 160
14.2.3.4.3.7. Particle Mass Flow .................................................................................... 160
14.2.3.4.3.8. Particle Diameter Distribution ................................................................... 160
14.2.3.4.3.9. Heat Transfer ............................................................................................ 160
xii
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
14.2.3.4.3.10. Component Details ................................................................................. 160
14.2.3.5. Fluid Values for Outlets .............................................................................................. 160
14.2.3.6. Fluid Values for Walls .................................................................................................. 160
14.2.3.6.1. Particle Tracking Settings for Walls ..................................................................... 160
14.2.3.6.2. Settings for Particle-Wall Interaction .................................................................. 161
14.2.3.7. Fluid Values for Interfaces ........................................................................................... 161
14.2.3.7.1. Fluid-Solid Interface, Fluid Side .......................................................................... 161
14.2.3.7.2. Fluid-Fluid and Periodic Interfaces ..................................................................... 162
14.2.4. Boundary Solid Values Tab .................................................................................................. 162
14.2.4.1. Heat Transfer ............................................................................................................. 162
14.2.4.1.1. Adiabatic .......................................................................................................... 162
14.2.4.1.2. Fixed Temperature ............................................................................................ 162
14.2.4.1.3. Heat Flux .......................................................................................................... 162
14.2.4.1.4. Heat Transfer Coefficient ................................................................................... 162
14.2.4.1.5. Conservative Interface Flux ................................................................................ 162
14.2.4.2. Additional Variables ................................................................................................... 163
14.2.5. Boundary Sources Tab ........................................................................................................ 163
14.2.6. Boundary Plot Options Tab ................................................................................................. 163
14.2.6.1. Boundary Contour ..................................................................................................... 163
14.2.6.2. Boundary Vector ........................................................................................................ 163
14.3. Interface Boundary Conditions .................................................................................................... 163
14.4. Symmetry Boundary Conditions .................................................................................................. 164
14.5. Working with Boundary Conditions ............................................................................................. 164
14.5.1. Boundary Condition Visualization ....................................................................................... 164
14.5.2. Profile Data and CEL Functions ............................................................................................ 164
14.5.2.1. Types of Discrete Profiles ............................................................................................ 164
14.5.2.2. Profile Data Format .................................................................................................... 165
14.5.2.3. Multiphase Boundary Condition Example ................................................................... 166
15. Initialization ...................................................................................................................................... 167
15.1. Using the User Interface .............................................................................................................. 167
15.1.1. Domain: Initialization Tab .................................................................................................... 167
15.1.1.1. Domain Initialization .................................................................................................. 168
15.1.2. Global Settings and Fluid Settings Tabs ............................................................................... 168
15.1.2.1. Coord Frame Check Box ............................................................................................. 168
15.1.2.1.1. Coord Frame Check Box: Coord Frame ................................................................ 168
15.1.2.2. Frame Type Check Box ............................................................................................... 168
15.1.2.2.1. Frame Type ....................................................................................................... 168
15.1.2.3. Initial Conditions: Velocity Type .................................................................................. 168
15.1.2.4. Initial Conditions: Cartesian Velocity Components ....................................................... 169
15.1.2.4.1. Option .............................................................................................................. 169
15.1.2.4.2. Velocity Scale Check Box ................................................................................... 169
15.1.2.4.2.1. Velocity Scale Check Box: Value ................................................................. 169
15.1.2.4.3. U, V, W ............................................................................................................... 169
15.1.2.5. Initial Conditions: Cylindrical Velocity Components ..................................................... 169
15.1.2.5.1. Option .............................................................................................................. 169
15.1.2.5.2. Velocity Scale Check Box ................................................................................... 169
15.1.2.5.3. Axial Component, Radial Component, Theta Component .................................... 170
15.1.2.6. Initial Conditions: Static Pressure ................................................................................ 170
15.1.2.6.1. Option .............................................................................................................. 170
15.1.2.6.2. Relative Pressure ............................................................................................... 170
15.1.2.7. Initial Conditions: Turbulence ..................................................................................... 170
15.1.2.7.1. Fractional Intensity ............................................................................................ 171
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xiii
ANSYS CFX-Pre User's Guide
15.1.2.7.2. Eddy Viscosity Ratio .......................................................................................... 171
15.1.2.7.3. Eddy Length Scale ............................................................................................. 171
15.1.2.7.4. Turbulence Kinetic Energy ................................................................................. 171
15.1.2.7.5. Turbulence Eddy Dissipation ............................................................................. 172
15.1.2.7.6. Turbulence Eddy Frequency .............................................................................. 172
15.1.2.7.7. Reynolds Stress Components ............................................................................ 172
15.1.2.8. Initial Conditions: Temperature ................................................................................... 172
15.1.2.9. Initial Conditions: Radiation Intensity .......................................................................... 173
15.1.2.9.1. Option .............................................................................................................. 173
15.1.2.10. Initial Conditions: Mixture Fraction ........................................................................... 173
15.1.2.10.1. Option ............................................................................................................ 173
15.1.2.10.2. Mixture Fraction .............................................................................................. 173
15.1.2.11. Initial Conditions: Mixture Fraction Variance .............................................................. 173
15.1.2.11.1. Option ............................................................................................................ 173
15.1.2.11.2. Mix. Fracn. Variance .......................................................................................... 174
15.1.2.12. Initial Conditions: Component Details ....................................................................... 174
15.1.2.12.1. List Box ........................................................................................................... 174
15.1.2.12.2. [component name]: Option ............................................................................. 174
15.1.2.12.3. [component name]: Mass Fraction ................................................................... 174
15.1.2.13. Initial Conditions: Additional Variable Details ............................................................ 174
15.1.2.14. Fluid Specific Initialization ........................................................................................ 174
15.1.2.15. Fluid Specific Initialization: List Box ........................................................................... 174
15.1.2.16. Fluid Specific Initialization: [fluid name] Check Box .................................................... 174
15.1.2.17. Fluid Specific Initialization: [fluid name] Check Box: Initial Conditions ........................ 175
15.1.2.17.1. Velocity Type ................................................................................................... 175
15.1.2.17.2. Volume Fraction: Option .................................................................................. 175
15.1.2.17.3. Volume Fraction: Volume Fraction .................................................................... 175
15.1.2.18. Solid Specific Initialization ........................................................................................ 175
15.1.2.19. Solid Specific Initialization: List Box ........................................................................... 175
15.1.2.20. Solid Specific Initialization: [solid name] Check Box ................................................... 175
16. Source Points ..................................................................................................................................... 177
16.1. Basic Settings Tab ........................................................................................................................ 177
16.2. Sources Tab ................................................................................................................................. 177
16.2.1. Single-Phase Fluid Sources ................................................................................................. 177
16.2.1.1. Component Mass Fractions ........................................................................................ 178
16.2.1.2. Additional Variables ................................................................................................... 178
16.2.1.3. Continuity ................................................................................................................. 178
16.2.1.3.1. Continuity Option ............................................................................................. 178
16.2.1.3.2. Additional Variables .......................................................................................... 178
16.2.1.3.3. Component Mass Fractions ............................................................................... 178
16.2.1.3.4. Temperature ..................................................................................................... 178
16.2.1.3.5. Velocity ............................................................................................................. 179
16.2.1.4. Energy ....................................................................................................................... 179
16.2.1.5. Turbulence Eddy Dissipation or Turbulence Kinetic Energy .......................................... 179
16.2.2. Multiphase Bulk Sources ..................................................................................................... 179
16.2.3. Multiplying Sources by Porosity .......................................................................................... 179
16.3. Fluid Sources Tab ........................................................................................................................ 179
16.4. Sources in Solid Domains ............................................................................................................ 179
16.5. Source Points and Mesh Deformation .......................................................................................... 180
17. Subdomains ...................................................................................................................................... 181
17.1. Creating New Subdomains .......................................................................................................... 181
17.2. The Subdomains Tab ................................................................................................................... 182
xiv
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
17.3. Basic Settings Tab ........................................................................................................................ 182
17.3.1. Location ............................................................................................................................. 182
17.3.2. Coordinate Frame ............................................................................................................... 182
17.4. Sources Tab ................................................................................................................................. 182
17.4.1. Single-Phase Fluid Sources ................................................................................................. 182
17.4.1.1. Momentum Source/Porous Loss ................................................................................. 183
17.4.1.2. Equation Sources ....................................................................................................... 183
17.4.1.2.1. Component Mass Fractions ............................................................................... 183
17.4.1.2.2. Additional Variables .......................................................................................... 183
17.4.1.2.3. Continuity ......................................................................................................... 184
17.4.1.2.4. Turbulence Quantities ....................................................................................... 184
17.4.1.2.5. Energy .............................................................................................................. 185
17.4.2. Bulk Sources for Multiphase Simulations ............................................................................. 185
17.4.3. Multiplying Sources by Porosity .......................................................................................... 185
17.5. Fluids Tab .................................................................................................................................... 185
17.5.1. Particle Absorption ............................................................................................................. 185
17.6. Mesh Motion .............................................................................................................................. 185
18. Rigid Bodies ...................................................................................................................................... 187
18.1. Rigid Body User Interface ............................................................................................................ 187
18.1.1. Insert Rigid Body Dialog Box ............................................................................................... 187
18.1.2. Basic Settings Tab ............................................................................................................... 188
18.1.2.1. Mass .......................................................................................................................... 188
18.1.2.2. Location .................................................................................................................... 188
18.1.2.3. Coord Frame .............................................................................................................. 188
18.1.2.4. Mass Moment of Inertia ............................................................................................. 189
18.1.3. Dynamics Tab ..................................................................................................................... 189
18.1.3.1. External Force Definitions .......................................................................................... 189
18.1.3.2. External Torque Definitions ........................................................................................ 190
18.1.3.3. Degrees of Freedom .................................................................................................. 191
18.1.3.3.1. Translational Degrees of Freedom ...................................................................... 191
18.1.3.3.2. Rotational Degrees of Freedom ......................................................................... 191
18.1.3.4. Gravity ...................................................................................................................... 191
18.1.4. Initial Conditions Tab .......................................................................................................... 191
18.1.4.1. Center of Mass ........................................................................................................... 192
18.1.4.2. Linear Velocity ........................................................................................................... 192
18.1.4.3. Angular Velocity ........................................................................................................ 192
18.1.4.4. Linear Acceleration .................................................................................................... 192
18.1.4.5. Angular Acceleration ................................................................................................. 192
19. Units and Dimensions ....................................................................................................................... 193
19.1. Units Syntax ................................................................................................................................ 193
19.2. Using Units in CFX-Pre ................................................................................................................. 194
19.2.1. Units Commonly Used in CFX .............................................................................................. 194
19.2.2. Defining Your Own Units .................................................................................................... 197
19.3. Setting the Solution Units ........................................................................................................... 197
20. Solver Control .................................................................................................................................... 199
20.1. Basic Settings Tab ........................................................................................................................ 199
20.1.1. Basic Settings: Common ..................................................................................................... 199
20.1.1.1. Advection Scheme ..................................................................................................... 199
20.1.1.2. Turbulence Numerics ................................................................................................. 199
20.1.1.3. Convergence Criteria ................................................................................................. 200
20.1.1.4. Elapsed Wall Clock Time Control ................................................................................. 200
20.1.1.5. Interrupt Control ........................................................................................................ 200
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xv
ANSYS CFX-Pre User's Guide
20.1.1.5.1. List Box ............................................................................................................. 200
20.1.1.5.1.1. [Interrupt Condition Name] ....................................................................... 200
20.1.1.6. Junction Box Routine ................................................................................................. 200
20.1.2. Basic Settings for Steady State Simulations .......................................................................... 201
20.1.2.1. Convergence Control: Min. Iterations .......................................................................... 201
20.1.2.2. Convergence Control: Max. Iterations .......................................................................... 201
20.1.2.3. Convergence Control: Fluid Timescale Control ............................................................ 201
20.1.2.4. Solid Timescale Control .............................................................................................. 201
20.1.3. Basic Settings for Transient Simulations ............................................................................... 201
20.1.3.1. Transient Scheme ...................................................................................................... 201
20.1.3.2. Convergence Control ................................................................................................. 201
20.1.3.2.1. Min. Coeff. Loops ............................................................................................... 201
20.1.3.2.2. Max. Coeff. Loops ............................................................................................... 202
20.1.3.2.3. Fluid Timescale Control ..................................................................................... 202
20.1.4. Immersed Solid Control ...................................................................................................... 202
20.2. Equation Class Settings Tab ......................................................................................................... 203
20.3. External Coupling Tab ................................................................................................................. 204
20.4. Particle Control Tab ..................................................................................................................... 204
20.5. Rigid Body Control Tab ................................................................................................................ 204
20.6. Advanced Options Tab ................................................................................................................ 207
21. Output Control .................................................................................................................................. 213
21.1. User Interface ............................................................................................................................. 213
21.1.1. Results Tab ......................................................................................................................... 213
21.1.1.1. Option ....................................................................................................................... 213
21.1.1.2. File Compression ....................................................................................................... 214
21.1.1.3. Output Variable List ................................................................................................... 214
21.1.1.4. Output Equation Residuals Check Box ........................................................................ 214
21.1.1.5. Output Boundary Flows Check Box ............................................................................. 214
21.1.1.6. Output Variable Operators Check Box ......................................................................... 214
21.1.1.7. Extra Output Variables List ......................................................................................... 214
21.1.1.8. Output Particle Boundary Vertex Fields Check Box ...................................................... 214
21.1.2. Backup Tab ......................................................................................................................... 214
21.1.2.1. List Box ...................................................................................................................... 214
21.1.2.2. [Backup Results Name] ............................................................................................... 214
21.1.2.2.1. Option .............................................................................................................. 214
21.1.2.2.2. File Compression ............................................................................................... 215
21.1.2.2.3. Output Variables List ......................................................................................... 215
21.1.2.2.4. Output Equation Residuals Check Box ............................................................... 215
21.1.2.2.5. Output Boundary Flows Check Box .................................................................... 215
21.1.2.2.6. Output Variable Operators Check Box ................................................................ 215
21.1.2.2.7. Extra Output Variables List ................................................................................. 215
21.1.2.2.8. Output Particle Boundary Vertex Fields Check Box ............................................. 215
21.1.2.2.9. Include Tracks of One-way Coupled Particles Check Box ..................................... 215
21.1.2.2.10. Output Frequency: Option ............................................................................... 215
21.1.3. Transient Results Tab .......................................................................................................... 215
21.1.3.1. List Box ...................................................................................................................... 215
21.1.3.2. [Transient Results Name] ............................................................................................ 216
21.1.3.2.1. Option .............................................................................................................. 216
21.1.3.2.2. File Compression ............................................................................................... 216
21.1.3.2.3. Output Variables List ......................................................................................... 216
21.1.3.2.4. Include Mesh .................................................................................................... 216
21.1.3.2.5. Output Equation Residuals Check Box ............................................................... 216
xvi
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
21.1.3.2.6. Output Boundary Flows Check Box .................................................................... 216
21.1.3.2.7. Output Variable Operators Check Box ................................................................ 216
21.1.3.2.8. Extra Output Variables List ................................................................................. 216
21.1.3.2.9. Output Particle Boundary Vertex Fields Check Box ............................................. 216
21.1.3.2.10. Output Frequency ........................................................................................... 216
21.1.3.3. Transient Blade Row Results ....................................................................................... 216
21.1.4. Transient Statistics Tab ........................................................................................................ 217
21.1.4.1. List Box ...................................................................................................................... 217
21.1.4.2. [Transient Statistics Name] ......................................................................................... 218
21.1.4.2.1. Option .............................................................................................................. 218
21.1.4.2.2. Output Variables List ......................................................................................... 218
21.1.4.2.3. Start Iteration List Check Box ............................................................................. 218
21.1.4.2.3.1. Start Iteration List Check Box: Start Iteration List ........................................ 218
21.1.4.2.4. Stop Iteration List Check Box ............................................................................. 218
21.1.4.2.4.1. Stop Iteration List Check Box: Stop Iteration List ........................................ 219
21.1.5. Monitor Tab ........................................................................................................................ 219
21.1.5.1. Monitor Objects Check Box ........................................................................................ 219
21.1.5.1.1. Monitor Coeff. Loop Convergence ...................................................................... 219
21.1.5.1.2. Monitor Balances: Option .................................................................................. 219
21.1.5.1.3. Monitor Forces: Option ...................................................................................... 219
21.1.5.1.4. Monitor Residuals: Option ................................................................................. 220
21.1.5.1.5. Monitor Totals: Option ....................................................................................... 220
21.1.5.1.6. Monitor Particles: Option ................................................................................... 220
21.1.5.1.7. Efficiency Output Check Box .............................................................................. 220
21.1.5.1.7.1. Inflow Boundary ....................................................................................... 220
21.1.5.1.7.2. Outflow Boundary .................................................................................... 220
21.1.5.1.7.3. Efficiency Type .......................................................................................... 220
21.1.5.1.7.4. Efficiency Calculation Method ................................................................... 221
21.1.5.1.8. Monitor Points And Expressions List Box ............................................................ 221
21.1.5.1.8.1. Monitor Points and Expressions: [Monitor Name]: Option ........................... 221
21.1.5.1.8.2. Monitor Points and Expressions: [Monitor Name]: Output Variables List ...... 221
21.1.5.1.8.3. Monitor Points and Expressions: [Monitor Name]: Cartesian Coordinates .... 221
21.1.5.1.8.4. Monitor Points and Expressions: [Monitor Name]: Cylindrical Coordinates ............................................................................................................................ 222
21.1.5.1.8.5. Monitor Points and Expressions: [Monitor Name]: Expression Value ............ 222
21.1.5.1.8.6. Monitor Points and Expressions: [Monitor Name]: Coord Frame Check
Box ............................................................................................................................. 222
21.1.5.1.8.7. Monitor Points and Expressions: [Monitor Name]: Coord Frame Check Box:
Coord Frame ............................................................................................................... 222
21.1.5.1.8.8. Monitor Points and Expressions: [Monitor Name]: Domain Name Check
Box ............................................................................................................................. 222
21.1.5.1.8.9. Monitor Points and Expressions: [Monitor Name]: Domain Name Check Box:
Domain Name ............................................................................................................ 222
21.1.5.1.9. Radiometer: Frame Overview ............................................................................. 222
21.1.5.1.10. Radiometer: List Box ........................................................................................ 223
21.1.5.1.10.1. Radiometer: [Radiometer Name]: Option ................................................. 223
21.1.5.1.10.2. Radiometer: [Radiometer Name]: Cartesian Coordinates .......................... 223
21.1.5.1.10.3. Radiometer: [Radiometer Name]: Temperature ......................................... 223
21.1.5.1.10.4. Radiometer: [Radiometer Name]: Quadrature Points ................................ 223
21.1.5.1.10.5. Radiometer: [Radiometer Name]: Coord Frame Check Box ........................ 223
21.1.5.1.10.6. Radiometer: [Radiometer Name]: Coord Frame Check Box: Coord
Frame ......................................................................................................................... 223
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xvii
ANSYS CFX-Pre User's Guide
21.1.5.1.10.7. Radiometer: [Radiometer Name]: Diagnostic Output Level Check Box ...... 223
21.1.5.1.10.8. Radiometer: [Radiometer Name]: Diagnostic Output Level Check Box: Diagnostic Output Level .................................................................................................. 223
21.1.5.1.10.9. Radiometer: [Radiometer Name]: Direction: Option .................................. 223
21.1.5.1.10.10. Radiometer: [Radiometer Name]: Direction: X Component,Y Component,
Z Component ............................................................................................................. 224
21.1.6. Particles Tab ....................................................................................................................... 224
21.1.6.1. Particle Track File Check Box ....................................................................................... 224
21.1.6.1.1. Option .............................................................................................................. 224
21.1.6.1.2. Track Positions Check Box .................................................................................. 225
21.1.6.1.3. Track Positions Check Box: Track Positions .......................................................... 225
21.1.6.1.4. Interval ............................................................................................................. 225
21.1.6.1.5. Track Distance Spacing ...................................................................................... 225
21.1.6.1.6. Track Time Spacing ............................................................................................ 225
21.1.6.1.7. Track Printing Interval Check Box ....................................................................... 225
21.1.6.1.8. Track Printing Interval Check Box: Interval .......................................................... 226
21.1.6.1.9. Keep Track File Check Box .................................................................................. 226
21.1.6.1.10. Track File Format Check Box ............................................................................. 226
21.1.6.1.11. Track File Format Check Box: Track File Format .................................................. 226
21.1.6.2. Transient Particle Diagnostics ..................................................................................... 227
21.1.6.3. Transient Particle Diagnostics: List Box ........................................................................ 227
21.1.6.4. Transient Particle Diagnostics: [Transient Particle Diagnostics Name] ........................... 227
21.1.6.4.1. Option .............................................................................................................. 227
21.1.6.4.2. Particles List ...................................................................................................... 227
21.1.6.4.3. Spray Mass Frac. ................................................................................................ 227
21.1.6.4.4. Penetration Origin and Direction: Option ........................................................... 227
21.1.6.4.5. Penetration Origin and Direction: Injection Center ............................................. 227
21.1.6.4.6. Penetration Origin and Direction: Injection Direction ......................................... 227
21.1.6.4.6.1. Option ..................................................................................................... 227
21.1.6.4.7. Axial Penetration: Option ................................................................................... 227
21.1.6.4.8. Radial Penetration: Option ................................................................................. 228
21.1.6.4.9. Normal Penetration: Option ............................................................................... 228
21.1.6.4.10. Spray Angle: Option ......................................................................................... 228
21.1.6.4.10.1. Spray Angle: Spray Radius at Penetration Origin Check Box ...................... 228
21.1.6.4.10.2. Spray Angle: Spray Radius at Penetration Origin Check Box: Spray Radius ............................................................................................................................... 228
21.1.7. Export Results Tab .............................................................................................................. 228
21.1.7.1. List Box ...................................................................................................................... 228
21.1.7.2. [Export Name]: Export Format .................................................................................... 229
21.1.7.2.1. Filename Prefix Check Box ................................................................................. 229
21.1.7.2.2. Filename Prefix Check Box: Filename Prefix ........................................................ 229
21.1.7.3. [Export Name]: Export Frequency ............................................................................... 229
21.1.7.3.1. Option .............................................................................................................. 229
21.1.7.4. [Export Name]: Export Surface .................................................................................... 229
21.1.7.4.1. List Box ............................................................................................................. 229
21.1.7.4.2. [Export Surface Name]: Option .......................................................................... 229
21.1.7.4.3. [Export Surface Name]: Output Boundary List .................................................... 229
21.1.7.4.4. [Export Surface Name]: Output Variables List ...................................................... 230
21.1.7.4.5. [Export Surface Name]: Output Nodal Area Vectors Check Box ............................ 230
21.1.8. Common Settings .............................................................................................................. 230
21.1.8.1. Option ....................................................................................................................... 230
21.1.8.2. File Compression ....................................................................................................... 230
xviii
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
21.1.8.3. Output Variables List .................................................................................................. 231
21.1.8.4. Output Equation Residuals Check Box ........................................................................ 231
21.1.8.5. Output Boundary Flows Check Box ............................................................................. 231
21.1.8.6. Output Variable Operators Check Box ......................................................................... 231
21.1.8.7. Output Particle Boundary Vertex Fields Check Box ...................................................... 231
21.1.8.8. Output Frequency Options ........................................................................................ 232
21.1.8.8.1. Timestep Interval .............................................................................................. 232
21.1.8.8.2. Timestep List ..................................................................................................... 232
21.1.8.8.3. Time Interval ..................................................................................................... 232
21.1.8.8.4. Time List ........................................................................................................... 232
21.1.8.8.5. Every Timestep .................................................................................................. 232
21.1.8.8.6. Every Iteration ................................................................................................... 232
21.1.8.8.7. Iteration Interval ............................................................................................... 232
21.1.8.8.8. Iteration List ...................................................................................................... 232
21.1.8.8.9. Wall Clock Time Interval ..................................................................................... 232
21.1.8.8.10. Coupling Step Interval ..................................................................................... 233
21.1.8.8.11. Every Coupling Step ........................................................................................ 233
21.1.8.8.12. None ............................................................................................................... 233
21.2. Working with Output Control ...................................................................................................... 233
21.2.1. Working with Transient Statistics ......................................................................................... 233
21.2.1.1. Statistic Initialization and Accumulation ..................................................................... 233
21.2.1.2. Statistics as Variable Operators ................................................................................... 234
21.2.1.3. Using Statistics with Transient Rotor-Stator Cases ....................................................... 235
21.2.2. Working with Monitors ....................................................................................................... 235
21.2.2.1. Setting up Monitors ................................................................................................... 235
21.2.2.2. Transient/ Mesh Deformation Runs ............................................................................. 235
21.2.2.3. Output Information ................................................................................................... 235
21.2.2.4. Expression ................................................................................................................. 236
21.2.2.5. Viewing Monitor Values during a Run ......................................................................... 236
21.2.2.6. Viewing Monitor Point Values after a Run .................................................................... 236
21.2.3. Working with Export Results ............................................................................................... 237
21.2.3.1. File Naming Conventions ........................................................................................... 237
21.2.3.2. Propagating Older Time Step Values ........................................................................... 237
21.2.3.3. Output Boundary List and Output Region Naming ...................................................... 237
21.2.3.4. Output Variables List .................................................................................................. 238
22. Transient Blade Row Models ............................................................................................................. 239
22.1. Inserting a New Transient Blade Row Models Object .................................................................... 239
22.2. Transient Blade Row Models Tab .................................................................................................. 239
22.2.1. Transient Blade Row Model Settings .................................................................................... 239
22.2.1.1. Time Transformation Disturbance Settings ................................................................. 240
22.2.1.2. Fourier Transformation Disturbance Settings .............................................................. 241
22.2.2. Transient Details ................................................................................................................. 242
23. Mesh Adaption .................................................................................................................................. 245
23.1. Overview .................................................................................................................................... 245
23.2. Setting Up Mesh Adaption .......................................................................................................... 246
23.3. The Details View for Mesh Adaption ............................................................................................. 247
23.3.1. Basic Settings Tab ............................................................................................................... 248
23.3.1.1. Region List ................................................................................................................. 248
23.3.1.2. Save Intermediate Files .............................................................................................. 248
23.3.1.3. Adaption Criteria ....................................................................................................... 248
23.3.1.3.1. Variables List ..................................................................................................... 248
23.3.1.3.2. Max. Num. Steps ................................................................................................ 248
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xix
ANSYS CFX-Pre User's Guide
23.3.1.3.3. Option .............................................................................................................. 249
23.3.1.4. Adaption Method ...................................................................................................... 249
23.3.1.4.1. Option .............................................................................................................. 249
23.3.1.4.2. Minimum Edge Length ...................................................................................... 249
23.3.1.5. Adaption Convergence Criteria .................................................................................. 249
23.3.2. Advanced Options Tab ........................................................................................................ 249
23.3.2.1. Node Alloc. Param. ..................................................................................................... 250
23.3.2.2. Number of Levels ....................................................................................................... 250
23.4. Advanced Topic: Adaption with 2D Meshes .................................................................................. 250
24. Expert Control Parameters ................................................................................................................ 253
24.1. Modifying Expert Control Parameters .......................................................................................... 253
25. Coordinate Frames ............................................................................................................................ 255
25.1. Creating a New Coordinate Frame ............................................................................................... 255
25.2. Coordinate Frame Basic Settings Tab ........................................................................................... 255
25.2.1. Coordinate Frame: Option ................................................................................................... 256
25.2.1.1. Point and Normal ....................................................................................................... 256
25.2.1.2. Axis Points ................................................................................................................. 256
25.2.2. Coordinate Frame: Centroid ................................................................................................ 256
25.2.2.1. Location .................................................................................................................... 256
25.2.2.2. Centroid Type ............................................................................................................ 256
25.2.3. Coordinate Frame: Direction ............................................................................................... 257
25.2.3.1. Invert Normal Axis Direction Check Box ...................................................................... 257
25.2.3.2. Point on Reference Plane 1-3 Check Box ..................................................................... 257
25.2.3.3. Point on Reference Plane 1-3 Check Box: Coordinate ................................................... 257
25.2.4. Coord Frame Type .............................................................................................................. 257
25.2.5. Reference Coord Frame ...................................................................................................... 257
25.2.6. Origin ................................................................................................................................ 257
25.2.7. Z-Axis Point ........................................................................................................................ 258
25.2.8. X-Z Plane Point ................................................................................................................... 258
25.2.9. Frame Motion Settings ....................................................................................................... 258
25.2.10. Visibility Check Box ........................................................................................................... 258
26. Materials and Reactions .................................................................................................................... 259
26.1. Materials ..................................................................................................................................... 259
26.1.1. Library Materials ................................................................................................................. 259
26.1.2. Material Details View: Common Settings ............................................................................. 260
26.1.2.1. Option ....................................................................................................................... 260
26.1.2.2. Material Group .......................................................................................................... 260
26.1.2.2.1. User .................................................................................................................. 260
26.1.2.2.2. Air Data ............................................................................................................ 261
26.1.2.2.3. CHT Solids ......................................................................................................... 261
26.1.2.2.4. Calorically Perfect Ideal Gases ............................................................................ 261
26.1.2.2.5. Constant Property Gases / Liquids ..................................................................... 261
26.1.2.2.6. Dry/Wet Redlich Kwong .................................................................................... 261
26.1.2.2.7. Dry/Wet Redlich Kwong RGP ............................................................................. 261
26.1.2.2.8. Dry/Wet Peng Robinson RGP ............................................................................. 261
26.1.2.2.9. Dry/Wet Soave Redlich Kwong RGP ................................................................... 262
26.1.2.2.10. Dry/Wet Steam ................................................................................................ 262
26.1.2.2.11. Gas Phase Combustion .................................................................................... 262
26.1.2.2.12. Interphase Mass Transfer ................................................................................. 262
26.1.2.2.13. Particle Solids .................................................................................................. 262
26.1.2.2.14. Soot ................................................................................................................ 262
26.1.2.2.15. Water Data ...................................................................................................... 262
xx
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
26.1.2.3. Material Description .................................................................................................. 262
26.1.2.4. Thermodynamic State ................................................................................................ 262
26.1.2.5. Coord Frame .............................................................................................................. 263
26.1.3. Material Details View: Pure Substance ................................................................................. 263
26.1.3.1. Basic Settings Tab ...................................................................................................... 263
26.1.3.2. Material Properties Tab .............................................................................................. 263
26.1.3.2.1. General Material ................................................................................................ 263
26.1.3.2.1.1. Equation of State - Value ........................................................................... 264
26.1.3.2.1.2. Equation of State - Ideal Gas ..................................................................... 264
26.1.3.2.1.3. Equation of State - Real Gas ...................................................................... 264
26.1.3.2.2. Table ................................................................................................................. 265
26.1.3.2.3. Table Generation ............................................................................................... 265
26.1.3.2.3.1. Minimum and Maximum Temperature ...................................................... 265
26.1.3.2.3.2. Minimum and Maximum Absolute Pressure .............................................. 265
26.1.3.2.3.3. Error Tolerance ......................................................................................... 266
26.1.3.2.3.4. Maximum Points ...................................................................................... 266
26.1.3.2.3.5. Pressure/Temperature Extrapolation ......................................................... 266
26.1.4. Material Details View: Fixed Composition Mixture ................................................................ 266
26.1.4.1. Basic Settings Tab ...................................................................................................... 266
26.1.4.2. Mixture Properties Tab ............................................................................................... 267
26.1.5. Material Details View: Variable Composition Mixture ............................................................ 267
26.1.5.1. Basic Settings Tab ...................................................................................................... 267
26.1.5.2. Mixture Properties Tab ............................................................................................... 267
26.1.6. Material Details View: Homogeneous Binary Mixture ........................................................... 267
26.1.6.1. Basic Settings Tab ...................................................................................................... 268
26.1.6.2. Saturation Properties Tab ........................................................................................... 268
26.1.6.2.1. General ............................................................................................................. 268
26.1.6.2.2. Table ................................................................................................................. 268
26.1.6.2.3. Real Gas ............................................................................................................ 268
26.1.6.2.4. Table Generation ............................................................................................... 268
26.1.7. Material Details View: Reacting Mixture ............................................................................... 268
26.1.7.1. Basic Settings Tab ...................................................................................................... 268
26.1.7.2. Mixture Properties Tab ............................................................................................... 269
26.1.8. Material Details View: Hydrocarbon Fuel .............................................................................. 269
26.1.8.1. Basic Settings Tab ...................................................................................................... 269
26.1.8.2. Proximate/ Ultimate Analysis Tab ................................................................................ 269
26.1.8.3. Mixture Materials Tab ................................................................................................. 269
26.2. Reactions .................................................................................................................................... 270
26.2.1. Basic Settings Tab ............................................................................................................... 270
26.2.2. Single Step ......................................................................................................................... 270
26.2.2.1. Single Step: Basic Settings .......................................................................................... 270
26.2.2.2. Single Step: Reactants ................................................................................................ 271
26.2.2.3. Single Step: Products ................................................................................................. 271
26.2.2.4. Single Step: Reaction Rates ......................................................................................... 271
26.2.3. Multiple Step ...................................................................................................................... 271
26.2.4. Flamelet Library ................................................................................................................. 272
26.2.5. Multiphase ......................................................................................................................... 272
26.2.5.1. Multiphase: Basic Settings .......................................................................................... 272
26.2.5.2. Multiphase: Reactants ................................................................................................ 272
26.2.5.3. Multiphase: Products ................................................................................................. 272
26.2.5.4. Multiphase: Multiphase Reactions .............................................................................. 273
27. Additional Variables .......................................................................................................................... 275
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xxi
ANSYS CFX-Pre User's Guide
27.1. User Interface ............................................................................................................................. 275
27.1.1. Insert Additional Variable Dialog Box .................................................................................. 275
27.1.2. Basic Settings Tab for Additional Variable Objects ................................................................ 275
27.1.2.1. Variable Type ............................................................................................................. 275
27.1.2.2. Units ......................................................................................................................... 276
27.1.2.3. Tensor Type ............................................................................................................... 276
27.1.3. Fluid Models and Fluid Specific Models Tabs for Domain Objects ......................................... 276
27.1.3.1. Additional Variable Details: List Box ............................................................................ 276
27.1.3.2. Additional Variable Details: [Additional Variable Name] Check Box ............................... 276
27.1.3.2.1. Option .............................................................................................................. 276
27.1.3.2.1.1. Transport Equation ................................................................................... 276
27.1.3.2.1.2. Diffusive Transport Equation ..................................................................... 276
27.1.3.2.1.3. Homogeneous Transport Equation ............................................................ 277
27.1.3.2.1.4. Homogeneous Diffusive Transport Equation ............................................. 277
27.1.3.2.1.5. Poisson Equation ...................................................................................... 277
27.1.3.2.1.6. Homogeneous Poisson Equation .............................................................. 277
27.1.3.2.1.7. Fluid Dependent ...................................................................................... 277
27.1.3.2.1.8. Algebraic Equation ................................................................................... 277
27.1.3.2.1.9. Vector Algebraic Equation ......................................................................... 277
27.1.3.2.2. Value ................................................................................................................ 277
27.1.3.2.3. Kinematic Diffusivity Check Box ......................................................................... 278
27.1.3.2.4. Kinematic Diffusivity Check Box: Kinematic Diffusivity ........................................ 278
27.1.3.2.5. AV Properties for Fluid: Frame Overview ............................................................. 278
27.1.3.2.6. AV Properties for Fluid: List Box .......................................................................... 278
27.1.3.2.7. AV Properties for Fluid: [Fluid Name] Check Box .................................................. 278
27.1.3.2.8. AV Properties for Fluid: [Fluid Name] Check Box: Kinematic Diffusivity ................. 278
27.1.3.2.9. Vector xValue, Vector yValue, and Vector zValue .................................................. 279
27.1.4. Boundary Details and Fluid Values Tabs for Boundary Condition Objects .............................. 279
27.1.4.1. Additional Variables: List Box ...................................................................................... 279
27.1.4.2. Additional Variables: [Name] ....................................................................................... 279
27.1.4.2.1. Option .............................................................................................................. 279
27.1.4.2.2. Value ................................................................................................................ 280
27.1.4.2.3. Flux .................................................................................................................. 280
27.1.4.2.4. Transfer Coefficient ........................................................................................... 280
27.2. Creating an Additional Variable ................................................................................................... 280
28. Expressions ....................................................................................................................................... 281
28.1. Expressions Workspace ............................................................................................................... 281
28.1.1. Definition ........................................................................................................................... 282
28.1.2. Plot .................................................................................................................................... 283
28.1.3. Evaluate ............................................................................................................................. 283
28.2. Creating an Expression ................................................................................................................ 283
28.3. Modifying an Expression ............................................................................................................. 284
28.4. Importing or Exporting an Expression .......................................................................................... 284
28.4.1. Importing CCL Expressions ................................................................................................. 284
28.4.2. Exporting CCL Expressions .................................................................................................. 284
29. User Functions ................................................................................................................................... 287
29.1. Interpolation Function ................................................................................................................ 287
29.1.1. One Dimensional Interpolation ........................................................................................... 287
29.1.1.1. Extended Minimum and Maximum ............................................................................ 288
29.1.2. Three Dimensional Interpolation ......................................................................................... 288
29.1.3. Importing Data from a File .................................................................................................. 289
29.1.4. Viewing and Editing Data Imported from a File .................................................................... 289
xxii
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
29.2. User Defined Function ................................................................................................................. 290
29.2.1. Function Name ................................................................................................................... 290
29.2.1.1. Defining Quantities with User CEL Functions .............................................................. 290
29.2.2. Argument Units .................................................................................................................. 290
29.2.3. Result Units ........................................................................................................................ 291
30. User Routines .................................................................................................................................... 293
30.1. User CEL Routines ....................................................................................................................... 293
30.1.1. Calling Name ...................................................................................................................... 294
30.1.2. Library Name and Library Path ............................................................................................ 294
30.2. Junction Box Routines ................................................................................................................. 295
30.3. Particle User Routines .................................................................................................................. 295
31. Simulation Control ............................................................................................................................ 297
32. Execution and Termination Control .................................................................................................. 299
32.1. Execution Control ....................................................................................................................... 299
32.1.1. Overview of Defining CFX-Solver Startup ............................................................................ 299
32.1.2. The Details View for Execution Control ................................................................................ 299
32.1.2.1. Solver Input File Name ............................................................................................... 300
32.1.2.2. Run Definition Tab ..................................................................................................... 300
32.1.2.2.1. Mesh Node Reordering ..................................................................................... 301
32.1.2.2.2. Optional Quitting CFX-Pre ................................................................................. 301
32.1.2.3. Partitioner Tab ........................................................................................................... 301
32.1.2.4. Solver Tab .................................................................................................................. 304
32.1.2.5. Interpolator Tab ......................................................................................................... 304
32.2. Termination Control .................................................................................................................... 304
32.2.1. Overview of Configuration Termination ............................................................................... 304
32.2.2. Details View for Termination Control ................................................................................... 305
33. Configurations .................................................................................................................................. 307
33.1. Overview of Defining a Configuration .......................................................................................... 307
33.2. The Details View for Configuration ............................................................................................... 308
33.2.1. General Settings Tab ........................................................................................................... 308
33.2.2. Remeshing Tab ................................................................................................................... 309
33.2.2.1. User Defined Remeshing ............................................................................................ 310
33.2.2.2. ANSYS ICEM CFD Replay Remeshing ........................................................................... 311
33.2.2.2.1. ICEM CFD Geometry Control .............................................................................. 311
33.2.2.2.2. ICEM CFD Mesh Control ..................................................................................... 312
33.2.2.2.3. Scalar Parameter ............................................................................................... 312
33.2.3. Run Definition Tab .............................................................................................................. 313
33.2.4. Partitioner Tab .................................................................................................................... 314
33.2.5. Solver Tab .......................................................................................................................... 316
33.2.6. Interpolator Tab .................................................................................................................. 317
34. Quick Setup Mode ............................................................................................................................. 319
34.1. Starting a New Case in Quick Setup Mode .................................................................................... 319
34.2. Simulation Definition Tab ............................................................................................................ 319
34.2.1. Simulation Data .................................................................................................................. 319
34.2.1.1. Problem Type ............................................................................................................ 320
34.2.2. Working Fluid ..................................................................................................................... 320
34.2.3. Mesh Data .......................................................................................................................... 320
34.3. Physics Definition ........................................................................................................................ 320
34.3.1. Analysis Type ...................................................................................................................... 321
34.3.2. Model Data ........................................................................................................................ 321
34.4. Boundary Definition .................................................................................................................... 321
34.5. Final Operations .......................................................................................................................... 322
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xxiii
ANSYS CFX-Pre User's Guide
35. Turbomachinery Mode ...................................................................................................................... 323
35.1. Starting a New Case in Turbo Mode ............................................................................................. 323
35.2. Navigation through Turbo Mode ................................................................................................. 324
35.3. Basic Settings .............................................................................................................................. 324
35.3.1. Machine Type ..................................................................................................................... 324
35.3.2. Axes ................................................................................................................................... 324
35.3.2.1. Coordinate Frame ...................................................................................................... 324
35.3.2.2. Rotational Axis ........................................................................................................... 324
35.3.2.3. Axis Visibility .............................................................................................................. 325
35.3.3. Analysis Type ...................................................................................................................... 325
35.4. Component Definition ................................................................................................................ 325
35.4.1. Component Selector .......................................................................................................... 325
35.4.2. Component Type ................................................................................................................ 325
35.4.3. Mesh File ............................................................................................................................ 325
35.4.4. Passages and Alignment ..................................................................................................... 326
35.4.4.1. Passages/Mesh .......................................................................................................... 326
35.4.4.2. Passages to Model ..................................................................................................... 326
35.4.4.3. Passages in 360 .......................................................................................................... 326
35.4.4.4. Theta Offset ............................................................................................................... 326
35.4.5. Available Volumes .............................................................................................................. 326
35.4.6. Region Information ............................................................................................................ 327
35.4.7. Wall Configuration .............................................................................................................. 327
35.5. Physics Definition ........................................................................................................................ 327
35.5.1. Fluid .................................................................................................................................. 327
35.5.2. Model Data ........................................................................................................................ 327
35.5.2.1. Reference Pressure ..................................................................................................... 327
35.5.2.2. Heat Transfer ............................................................................................................. 327
35.5.2.3. Turbulence ................................................................................................................ 327
35.5.3. Boundary Templates ........................................................................................................... 327
35.5.4. Interface ............................................................................................................................ 328
35.5.5. Solver Parameters ............................................................................................................... 328
35.5.5.1. Advection Scheme ..................................................................................................... 328
35.5.5.2. Convergence Control ................................................................................................. 328
35.5.5.3. Time Scale Option ...................................................................................................... 328
35.5.5.4. Max. Coeff. Loops ....................................................................................................... 328
35.6. Interface Definition ..................................................................................................................... 328
35.6.1. Type ................................................................................................................................... 329
35.7. Disturbance Definition ................................................................................................................ 329
35.7.1. Type ................................................................................................................................... 329
35.8. Boundary Definition .................................................................................................................... 330
35.8.1. Boundary Data ................................................................................................................... 330
35.8.2. Flow Specification/Wall Influence on Flow ........................................................................... 330
35.9. Final Operations .......................................................................................................................... 330
36. Library Objects .................................................................................................................................. 331
36.1. Boiling Water .............................................................................................................................. 331
36.2. Cavitating Water ......................................................................................................................... 332
36.3. Coal Combustion ........................................................................................................................ 332
36.4. Comfort Factors .......................................................................................................................... 332
36.5. Multigray Radiation ..................................................................................................................... 333
37. Command Editor Dialog Box ............................................................................................................. 335
37.1. Using the Command Editor ......................................................................................................... 335
37.2. Performing Command Actions .................................................................................................... 336
xxiv
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ANSYS CFX-Pre User's Guide
37.3. Using Power Syntax ..................................................................................................................... 336
Index ........................................................................................................................................................ 337
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xxv
xxvi
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 1: CFX-Pre Basics
CFX-Pre is the physics-definition pre-processor for ANSYS CFX. You import meshes (which can be produced in a variety of mesh generation software packages) into CFX-Pre and select physical models1 to
be used in the CFD simulation. Files produced by CFX-Pre are sent to CFX-Solver.
This chapter describes:
1.1. Starting CFX-Pre
1.2. CFX-Pre Modes of Operation
1.3. Working with the CFX-Pre Interface
1.4. CFX-Pre File Types
If you want to start using CFX-Pre immediately, refer to the following CFX Tutorials:
•
"Simulating Flow in a Static Mixer Using CFX in Stand-alone Mode"
•
"Flow in a Static Mixer (Refined Mesh)"
•
"Flow in a Process Injection Mixing Pipe"
1.1. Starting CFX-Pre
When starting CFX-Pre for the first time, the default system font is obtained and, if it is deemed inappropriate for CFX-Pre, a dialog box appears that enables you to choose a new font. When a new font
is selected, it is stored for future sessions. For details, see Appearance (p. 48).
CFX-Pre can be started in different ways:
•
From within ANSYS Workbench choose Fluid Flow (CFX) from Toolbox > Analysis Systems or CFX
from Toolbox > Component Systems. In the Project Schematic, right-click on the Setup cell and select
Edit.
•
From the ANSYS CFX Launcher: set the working directory and then click CFX-Pre 14.0.
•
From the command line. The basic command is:
<CFXROOT>/bin/cfx5pre
The command line options are described in the next section.
Starting CFX-Pre from the Command Line
To start CFX-Pre from a command line, you must either:
1
•
Specify the full path to the executable (<CFXROOT>/bin/cfx5pre)
•
Append the path to the ANSYS CFX executables (<CFXROOT>/bin/) to your PATH.
For details on physical models, see Physical Models in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
1
Chapter 1: CFX-Pre Basics
–
On Windows, right-click the My Computer icon and select Properties. Click the Advanced tab, then
click Environment Variables. In the System variables section, edit PATH to include the path to
the ANSYS CFX executables; typically this will be something like:
C:\Program Files\ANSYS Inc\v140\CFX\bin;
–
On Linux/UNIX, edit your .<window_manager>rc file to include the path to the ANSYS CFX executables.
Once the PATH has been updated, the basic command is:
cfx5pre
•
Run the executable from the launcher Tools > Command Line (which has the path to the ANSYS CFX
executables built-in).
There are a number of optional command line flags, some of which are summarized in the following
table:
Argument
Alternative Form
Usage
Starts CFX-Pre in batch modea, running the session
file you enter as an argument.
-batch filename.pre
-display display
-d
Displays the graphical user interface on the X11
server display instead of using the X11 server
defined by the DISPLAY environment variable.
-gui
Starts CFX-Pre in graphical user interface (GUI)
mode. This is the default mode.
-line
Starts CFX-Pre in line interface mode.
-graphics ogl
-gr ogl
-graphics mesa
-gr mesa
Loads the named CFX-Solver input file after starting.
-def file
-session file
-s
Plays the named session file after starting.
Loads the named case file after starting.
-cfx file
-verbose
Specifies the graphics system as ogl or mesa. ogl is
the default.
-v
Specifying this option may result in additional output being sent to the standard output.
a
When launching CFX-Pre on a remote UNIX or Linux machine (though X, Exceed, and so on), the DISPLAY variable must be set to a valid
X display before running in batch mode.The display will typically be your local Windows, Linux, or UNIX machine.The remote machine must
have permission to connect to the display (for example, by use of the xhost command if the X display is on a UNIX/Linux machine).
To view a full list of command-line flags, execute:
cfx5pre -help
1.2. CFX-Pre Modes of Operation
When you select File > New Case to create a new simulation, CFX-Pre presents four different modes
of operations:
2
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with the CFX-Pre Interface
Figure 1.1 The New Case Dialog Box
•
General mode is the general-purpose mode for defining all types of CFD simulation. This mode uses
the general CFX-Pre interface, which is described in Working with the CFX-Pre Interface (p. 3).
•
Turbomachinery mode is a customized mode for defining turbomachinery simulations. For details, see
Turbomachinery Mode (p. 323).
•
Quick Setup mode greatly simplifies the physics setup for a simulation. Quick Setup mode is limited to
a single-domain and single-phase problems; more complex physics, such as multiphase, combustion,
radiation, advanced turbulence models, and so on are not available. You can, however, use Quick Setup
mode to get started, and then add more physics details later. For details, see Quick Setup Mode (p. 319).
•
Library Template mode provides a set of library files that are available with templates for specific physical problem definitions. In this mode you can easily define a complex physics problem by loading a
template file, importing a mesh, and defining specific problem data. For details, see Library Objects (p. 331).
1.3. Working with the CFX-Pre Interface
The CFX-Pre interface enables the easy definition of a simulation. The main components are the viewer
(to display and manipulate meshes), the workspaces (to define different aspects of the physics setup),
the physics message window, and the menus and tool bars (access to extra tools and utilities).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3
Chapter 1: CFX-Pre Basics
Figure 1.2 Sample CFX-Pre Interface
1.3.1. Viewer
The viewer displays imported geometries and meshes and enables manipulations and transformations
to be viewed. Information about boundary conditions, domains, point sources, and so on, is also displayed, and items can be picked directly from the Viewer.
CFX-Pre uses the same viewer as CFD-Post. Information on the generic CFX-Pre/CFD-Post viewer is
available in CFX-Pre 3D Viewer (p. 17). Many aspects of the viewer appearance can be customized, as
described in Options (p. 42).
1.3.2. CFX-Pre Workspace
The CFX-Pre workspace contains a tree view as well as various details views that are used during the
specification of mesh import, mesh transformation, physics, regions, materials, and expressions.
A powerful feature of CFX-Pre is automatic physics checking. Objects that contain inconsistent or incorrect
settings are highlighted in red. Detailed error messages are shown in the physics validation summary
window. For details, see Physics Message Window (p. 11).
4
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with the CFX-Pre Interface
1.3.2.1. Outline Tree View
The Outline tree view displays a summary of the physics that have been defined for the simulation.
The tree view window initially contains a default list of objects in a tree format.
The following topics are discussed in this section:
•
General Considerations (p. 5)
•
Outline Tree View Structure (p. 5)
•
Outline Tree View Shortcut Menu Commands (p. 7)
Tip
Typing Ctrl-F activates the search facility, which can be used to quickly locate an item in the
tree. Note that the search is case-sensitive and that the text box disappears after a few
seconds of inactivity.
1.3.2.1.1. General Considerations
When working with the tree view, note the following:
•
New objects are displayed in the tree as they are created.
•
Clicking on any object that is applied to a region will highlight that region in the viewer when highlighting is enabled (that is, when the Highlighting icon
see 3D Viewer Toolbar (p. 19).
is selected in the 3D Viewer toolbar). For details,
•
Objects shown in red contain incorrect physics definitions.
•
Right-click an object (or group selection of objects) to display the shortcut menu.
For details, see Outline Tree View Shortcut Menu Commands (p. 7).
1.3.2.1.2. Outline Tree View Structure
The Outline tab displays the tree view, which shows a summary of the current physics definition for a
simulation. The tree structure displayed reflects the structure used in the CFX Command Language
(CCL) for physics definition. You can select any object in the tree and double-click to gain direct access
to the appropriate tab to edit its settings. You can also right-click an object and display the CCL definition
of an object in the Command Editor dialog box, where it can be edited.
The remainder of this section describes the main areas in the Outline view.
Mesh
Provides access to all mesh operations in CFX-Pre. This includes mesh import, mesh transformations,
and the render/visibility properties of meshes in the viewer. Meshes generated in many other mesh
generation packages can be imported into CFX-Pre. For details, see Importing and Transforming
Meshes (p. 65).
Meshes that have been glued together are listed under Connectivity in the tree view.
Simulation
Enables you to define the one or more analyses of the simulation.
Optionally, you can open a copy of the Simulation branch in a separate tab.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
5
Chapter 1: CFX-Pre Basics
Analysis
Enables you to define and edit an analysis:
Analysis Type
Enables the specification of an analysis as steady state or transient, and whether it requires
coupling to an external solver. For details, see Analysis Type (p. 101).
Domains
Enables you to define and edit the type, properties and region of the fluid, porous or solid. For
details, see Domains (p. 105), Boundary Conditions (p. 149), Subdomains (p. 181) and Source
Points (p. 177).
Domain Interfaces
Enables you to define and edit the method of connecting meshes or domains together. For details,
see Domain Interfaces (p. 137).
Global Initialization
Enables you to set global initial conditions (across all domains). Domain specific initialization is
set through the domain forms. For details, see Initialization (p. 167).
Solver
Enables the defining and editing of Setting the Solution Units (p. 197), Solver Control (p. 199), Solver:
Expert Parameter (p. 57), Output Control (p. 213) and Mesh Adaption (p. 245).
Coordinate Frames
Creates and edits coordinate frames. A Cartesian coordinate frame exists by default, but other
Cartesian coordinate frames can be made. For details, see Coordinate Frames in the CFX-Solver
Modeling Guide and Coordinate Frames (p. 255).
Materials / Reactions
Creates, edits, and displays materials and reactions. Many different material types can be defined,
edited or imported. Specialist materials and reactions can be imported from external files, such as
the RGP (Real Gas Properties) file and Flamelet reaction files. For details, see Materials and Reactions (p. 259).
Expressions, Functions, and Variables
Used to create, edit and plot expressions, user functions, user routines, and Additional Variables. For
details, refer to the following sections:
•
Additional Variables (p. 275)
•
Expressions (p. 281)
•
User Functions (p. 287)
•
User Routines (p. 293)
Simulation Control
Enables you to set up the control of analyses in the simulation. This control is facilitated by defining
and editing one or more configurations as well as global solver execution control. For more information, see Solve (p. 47).
Case Options
The Graphics Style, Labels and Markers, and General options enable you to override the defaults for
the current simulation only — they will not be retained for future simulations. The default settings for
CFX-Pre are set in the Edit > Options dialog box — these settings are retained and take effect when a
new case is started. See CFX-Pre Options (p. 42) for a description of these settings.
6
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with the CFX-Pre Interface
Extensions
Enables you to access to any customized extensions available to CFX-Pre. For details, see CFX-Pre Extensions
Menu (p. 63).
1.3.2.1.2.1. Outline Tree View Shortcut Menu Commands
Right-clicking on any object in the tree view displays a shortcut menu. Double-clicking on an object
performs the default action for that object. Shortcut menu command descriptions follow:
Command
Description
Configuration
Simulation Control > Configurations > Insert > Configuration opens the
Configuration Editor.
Copy
The Copy command is usually combined with Paste to quickly replicate objects.
Define Connection
Mesh > Define Connection opens the Mesh Connections Editor.
Delete
Deletes the selected object. The physics for the simulation are checked after
objects are deleted. Objects containing invalid parameters are highlighted in
red in the tree view.
Delete All
Mesh
Deletes the mesh, but not the named areas in the Outline view. When this
happens, the Physics Message Window will show errors that say the named objects cannot be found. If you then import a new mesh that uses the same names
for objects, the names will be resolved and the errors will disappear.
Duplicate
Copies the definition of the selected object to a new object. You will be required
to enter a name for the duplicated object, which will then be created at the
same level (that is, for a boundary condition, the new boundary will be created
in the same domain as the initial object).
Edit
Opens the relevant tab where new parameters for the object can be entered.
In most casesa, you can also edit an object by double-clicking it in the tree view.
Edit In Command Editor
Opens the Command Editor dialog box and displays the CCL definition for the
highlighted object. You can edit the CCL directly to change the object definitiona.
For details, see Command Editor Dialog Box (p. 335).
Expand/Collapse SubBranches
Provides a fast way to navigate the tree view.
Export CCL
Opens the Export CCL dialog box, which is similar to the dialog box described
in Export Region Data, below.
Export Region Data
Opens the Export Region CCL dialog box, used to save the region data to a
.ccl file.
Glue Adjacent Meshes
If there are multiple mesh assemblies that have matched meshes, you can use
this option to try to glue them together. Select the assemblies in the tree view
(while holding down the Ctrl key).
Gluing can be useful to avoid setting up a GGI interface within a domain, but
does require that the meshes match exactly on the surfaces that are to be glued.
When you transform or copy multiple assemblies, each copy is not only glued
to its original assembly or to other copies, but also to any other assemblies that
are transformed or created. For more information, see Gluing Meshes Together (p. 88).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
7
Chapter 1: CFX-Pre Basics
Command
Description
Hide
Makes the active object invisible in the viewer. Hide has the same effect as
clearing the check box next to an object in the tree view.
Hide Interface Boundaries
Hides the interface boundaries in the Outline view.
Import CCL
Opens the Import CCL dialog box, which is similar to the dialog box described
in Import Region Data, below.
Import Mesh
Opens the Import Mesh dialog box. This is used to import a new mesh using
an appropriate file. For details, see Importing Meshes (p. 65).
Import Library Data
This command, available from the Materials branch in the tree view, is used
to add a new material to the simulation. Examples of such a material include
Methanol CH4O, Rubber, Water at 25 C, and many more.
Import Region Data
Opens the Import Region CCL dialog box. This is used to load region data from
a .ccl file.
Insert
Various objects are available for insertion, depending on which object is highlighted. All of the options available from this menu can also be accessed from
the Insert menu. For details, see CFX-Pre Insert Menu (p. 55).
Mesh Statistics
Opens the Mesh Statistics dialog box and provides a detailed information about
the active mesh. The Mesh Statistics dialog box can be invoked for one or more
assemblies and/or primitive 3D/2D regions. The data displayed includes the
number of nodes, elements, the number of each element type, and physical
extents of the mesh. The Maximum Edge Length Ratio is also calculated.
Paste
The Paste command is available when you have already used the Copy command
on an object.
To avoid producing objects with the same name, you are prompted to provide
a name when you paste the new object. For objects that contain a location
parameter (such as domains and boundary conditions), you will usually need to
edit the new object after pasting it to avoid multiple objects that reference the
same location.
If you are pasting a domain object, then you will need to edit each child object
in the domain that references a location. For example, you will need to change
the locations that boundary conditions reference so that they point to locations
in the new domain. You can simply delete a default domain boundary in this
situation; this will allow CFX-Pre to create a new default boundary for the domain
that references the correct locations.
Reload Mesh
Files
If any of the mesh regions become corrupted or are accidentally deleted, selecting
Reload Mesh Files reloads all mesh files used in the simulation. This command
cannot be used to insert a new mesh; do to so, select Import Mesh. For details,
see Reload Mesh Files Command (p. 34).
Note
This command is not required (and is not available) in CFX-Pre
launched from ANSYS Workbench.
8
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with the CFX-Pre Interface
Command
Description
Rename
Changes the selected object’s name.
Render
Enables you to change the appearance of almost any object. For example, a
boundary condition or domain interface can be displayed with a solid color, the
transparency of a domain can be altered, and so on.
Report Interface Summary
Invokes a message box that shows a summary of the interfaces and their types.
For details, see Mesh Connection Options in the CFX-Solver Modeling Guide.
Show/Hide
Makes the active object either visible (Show) or invisible (Hide) in the viewer.
Show and Hide have the same respective effects as selecting and clearing the
check box next to a specific object in the tree view.
Show Interface Boundaries
Shows the interface boundaries in the Outline view.
Start Solver
Enables you to access the Define Run, Run Solver, and Run Solver and Monitor
commands. These commands are also available from the main toolbar.
Transform
Mesh
Opens the Mesh Transformation Editor dialog box, allowing you to modify the
location of the active mesh through rotation, translation, or reflection. The mesh
can also be resized using a scaling method. For details, see Transform Mesh
Command (p. 82).
Use as Workbench Input
Parameter
Available when an expression is selected, this command allows the expression
to be used as a workbench input parameter.
View By
This command, available for the Mesh object, opens a new tab that presents a
detailed mesh information in one of two ways. Selecting View By > Source File
displays the mesh regions based on the mesh file provided, whereas View By
> Region Type organizes the areas of the mesh based on the defined 2D regions.
View in New
Tab
Simulation > View in New Tab enables you to view a copy of the contents of
the Simulation branch in a separate tab.
View in CFDPost
Prompts you to save a DEF file, then automatically starts CFD-Post with that file
loaded.
Write Solver
Input File
Has the same effect as clicking Write Solver Input File
or selecting Tools >
Solve > Write Solver Input File from the menu bar. For details, see Write Solver
Input File Command (p. 61).
a
An expression that is set as an input parameter in ANSYS Workbench cannot be edited in CFX-Pre or CFD-Post (as the results of such edits
are not passed to ANSYS Workbench) and will be grayed out. However, the expression can be declared to no longer be an input parameter
or it can be deleted.
1.3.2.2. Details View
Details view is a generic term for the editor pane that opens when you edit an object in the Outline
tree view. These editors appear on tabs beside the Outline tab and present the fields and controls that
define the object.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
9
Chapter 1: CFX-Pre Basics
Figure 1.3 Sample CFX-Pre Details View
The optional toggles provide you with the opportunity to view and, if desired, to override CFX-Pre default
settings. In the example above, selecting the Upper Courant Number option has made it possible to
see the default value for that setting; the white background indicates that you can the edit that value.
Most CFX-Pre settings have default values that will enable you to define an object or set a control as
easily as possible. If there is a setting that requires you to set a value, basic physics checking occurs
when you click OK or Apply on a details view and most missing settings are detected then. Complete
physics checking takes place when you attempt to write a solver file and all missing settings are detected
and reported at that time.
You use the Details view to define the properties of an object. The Details view contains one or more
tabs, depending on the type of object being defined.
Many properties can be set via a CEL expression. To enter an expression:
10
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with the CFX-Pre Interface
1.
Click in the field for a property.
2.
Click the Enter Expression icon that appears beside the field. This enables the field to accept an expression name.
3.
Either enter an expression definition directly, or type the name of an existing expression. You must
ensure that the expression evaluates to a value having appropriate units for the property that uses
the expression.
For details on CEL expressions, see Expressions (p. 281).
For CFX components in ANSYS Workbench, any CEL expression can be made into a parameterized CEL
expression by defining it as a Workbench input parameter. You can do this by creating an expression
and parameterize it by right-clicking it in the Expression editor. You can then use that expression as
the value of a property.
You can change a property from being specified by a Workbench input parameter. However, the corresponding CEL expression persists and can be managed by the Expression editor.
1.3.3. Physics Message Window
As you work through your simulation, CFX-Pre continually checks the physics definitions you have
specified. Whenever an action is carried out, the physics validator runs a check on the CCL definitions
of all the objects created up to that point. Physics checking is carried out by comparing the current
CCL data against library files such as RULES, VARIABLES and PHYSICS, which are known to contain
only valid physics specifications. If an inconsistency is found in the physics, the object with associated
error(s) is highlighted in red text in the tree view.
In addition to object name highlighting, the physics validation window displays all error types in the
simulation: global errors, physics errors and expression errors. The output in this window gives an explanation of each of the detected errors. Double-clicking on a red item or a maroon item (an expression
error) in the physics validation window will take you to the correct place in order to edit the object.
Global errors apply to the entire simulation and show errors that are not specific physics errors. Often
these errors show required objects that need to be defined to complete the simulation (for example,
initial conditions or a domain). They also show invalid referencing of regions in a simulation. In some
cases, the global errors offer a suggestion rather than being a definite error. For example, if you have
created two valid boundary conditions on one region, a global error will be shown (despite the fact
that the physics for both boundary conditions may be correct) because you cannot specify more than
one boundary condition on any given surface.
Physics errors (highlighted in red) involve an incorrect application of physics.
•
Global errors appear in blue text.
•
Specific physics errors appear in red text. You can double-click these to edit the object containing the
error.
There are two common situations when you are likely to encounter physics errors:
1.
CFX-Pre defines some objects, such as the Solver Control settings, by default. If you create a new
object that is not compatible with the default objects settings, the physics validation summary window
will show errors in the default object. This occurs when creating a solid domain because the default
Solver Control settings do not contain a solid time scale. These errors will disappear when you define
the Solver Control settings.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
11
Chapter 1: CFX-Pre Basics
2.
When changing the physics of an existing model. There are many instances where you might want to
change the description of your simulation. One particular situation is when you want to use the values
in a results file as the initial field for another run with different physics.
When a domain is modified, perhaps with new model options, you will receive errors or warnings
in the physics validation summary window if existing boundary conditions, initialization, solver
control, etc., need to be revisited and updated. This happens, for example, when the turbulence
model is changed from the laminar model to the − model and the boundary conditions for
the laminar case do not contain turbulence data (for example, at an Inlet). You should fix any such
errors before writing a CFX-Solver input file.
You should update boundary conditions if the number of Additional Variables has been increased,
or if the units for Additional Variable specifications have been changed.
If the simulation is set up correctly, there will not be any physics errors when you are ready to write
the CFX-Solver input file.
1.3.3.1. Physics Errors from Old .def/.res Files
When you load CFX-Solver input/results files from previous versions of ANSYS CFX, you may receive
error messages, despite the fact that the files can be run in the CFX-Solver. This is due to differences
in the previous CFX-Solver input files. In CFX-Pre, a more strict approach to CCL structure and content
has been implemented to ensure the integrity of the CCL made available to the CFX-Solver.
CFX-Pre performs some automatic updates when opening CFX-Solver input or results files from previous
versions of ANSYS CFX.
1.3.3.2. Physics Message Window Shortcut Menu Commands
Right-click on a message in the physics message window to perform the following functions:
Copy
Enables copying of the selected message.
Edit
Enables you to use the Details View to edit the object generating the error.
Auto Fix Physics
Enables you to attempt to correct inconsistent physics automatically. In many cases, you will find that
this fixes the problem without a need to change any settings on the form. Alternatively, you can use
the Details View to edit the object generating the error.
Viewing the type of error before performing auto fix is strongly recommended. For example, auto
fix cannot fix a domain with an incorrectly specified location. In effect, auto fix opens the default
layout of the panel and performs an apply. If you are unsure about auto fix, you should subsequently
open the form and verify that the settings are still valid for your problem. You should fix all physics
validation errors to ensure that the CFX-Solver input file runs in the solver. If any errors are found
when you attempt to write the CFX-Solver input file, a warning message is displayed giving you
the option to write the file anyway or cancel the operation.
Auto Fix All
Runs auto-fix on all objects that have physics validation errors.
Suppress this message
Suppress the selected message; a message summary is displayed instead.
12
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFX-Pre File Types
Suppress all messages
Suppresses all messages; message summaries are displayed instead. Note that messages generated
subsequently will not be suppressed.
Unsuppress all messages
Unsuppress all messages.
1.3.4. Menu Bar
The menu bar provides access to CFX-Pre functions. Some of these functions are also available from
the Toolbar (p. 13).
File Menu
Provides access to file operations including opening and saving simulations, as well as importing or exporting CCL. For details, see CFX-Pre File Menu (p. 31).
Edit Menu
Enables you to change the default options used by ANSYS CFX and undo/redo actions. For details, see
CFX-Pre Edit Menu (p. 41).
Note
Some options can be overridden for the current simulation; see Case Options in Outline
Tree View Structure (p. 5) for details.
Session Menu
Controls the recording and playing of session files. Session files are used to record a set of operations.
You can then play back a session file to quickly reproduce the same operations. For details, see CFX-Pre
Session Menu (p. 51).
Insert Menu
Enables you to create new objects such as domains or boundary conditions, or edit existing objects of
that type. For details, see CFX-Pre Insert Menu (p. 55).
Tools Menu
Provides access to tools such as command editor, macro calculator as well as quick setup and turbo
modes. For details, see CFX-Pre Tools Menu (p. 59)
Extensions Menu
Provides access to any customized extensions available to CFX-Pre. For details, see CFX-Pre Extensions
Menu (p. 63).
Help Menu
Provides access to the ANSYS CFX online help. You can access commonly used help pages directly including the master contents and the global search facility. For details, see Help On Help in the CFX Introduction.
1.3.5. Toolbar
The toolbar provides quick access to commonly used functions. The toolbar contains the most common
menu items and viewer controls. Holding the mouse pointer over a toolbar icon for a short period of
time displays the icon’s function.
1.4. CFX-Pre File Types
The following file types are used by or produced by CFX-Pre:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
13
Chapter 1: CFX-Pre Basics
Case Files (.cfx)
The case file contains the physics data, region definitions, and mesh information for the simulation and
is used by CFX-Pre as the 'database' for the simulation setup. The case file is generated when you save
a simulation in CFX-Pre. To re-open a simulation, select File > Open Case and pick a case file to open.
When you import a mesh into CFX-Pre, it passes through an import filter and is stored as part of
the case file. Therefore, once a mesh has been imported, the original mesh file is not required by
CFX-Pre. Additional information on importing meshes is available in Importing Meshes (p. 65).
The case file is a binary file and cannot be edited directly.
You can open cases on any supported platform, regardless of the platform on which they were
created.
Mesh Files
There are many types of mesh files that can be imported into CFX-Pre. For details, see Supported Mesh
File Types (p. 67).
CFX-Solver Input Files (.def, .mdef)
A CFX-Solver input file is created by CFX-Pre. The input file for a single configuration simulation (.def)
contains all physics and mesh data; the input file for multi-configuration simulations (.mdef) contains
global physics data only (that is, Library and Simulation Control CFX Command Language specifications).
An .mdef input file is supplemented by Configuration Definition (.cfg) files that:
•
Are located in a subdirectory that is named according to the base name of the input file
•
Contain local physics and mesh data.
Note
Use the -norun command line option (described in Command-Line Options and Keywords
for cfx5solve in the CFX-Solver Manager User's Guide) to merge global information into
the configuration definition files, and produce a CFX-Solver input file (.def) that can be
run by the CFX-Solver.
You can load a CFX-Solver input file back into CFX-Pre to recreate a simulation. CFX-Solver input
files from previous releases of ANSYS CFX can be loaded into CFX-Pre, although the physics definition
may have to be updated for such files. For details, see Physics Errors from Old .def/.res Files (p. 12).
CFX-Solver Results Files (.res, .mres, .trn, .bak)
Intermediate and final results files are created by the CFX-Solver:
•
Intermediate results files, which include transient and backup files (.trn and .bak, respectively)
are created while running an analysis.
•
Final results files for single and multi-configuration simulations (.res and .mres, respectively) are
written at the end of the simulation’s execution. For multi-configuration simulations, a configuration
result file (.res) is also created at the end of each configuration’s execution.
Each results file contains the following information as of the iteration or time step at which it is
written:
14
•
The physics data (that is, the CFX Command Language specifications)
•
All or a subset of the mesh and solution data.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFX-Pre File Types
CFX-Solver Backup Results Files (.bak)
A backup file (.bak) is created at your request, either by configuring the settings on the Backup tab
in Output Control in CFX-Pre, or by choosing to write a backup file while the run is in progress in the
CFX-Solver Manager.
CFX-Solver Transient Results Files (.trn)
A transient results file (.trn) is created at your request, by configuring the settings on the Output
Control > Trn Results tab in CFX-Pre.
CFX-Solver Error Results Files (.err)
An error results file (.err) is created when the CFX-Solver detects a failure and stops executing an
analysis. The .err file can be loaded into CFD-Post and treated the same way as a .bak file, but if the
CFX-Solver encounters another failure while writing the .err file, it may become corrupted and accurate
solutions cannot be guaranteed.
Session Files (.pre)
Session files are used by CFX-Pre to record CFX Command Language (CCL) commands executed during
a session. The commands can be played back at a later date to reproduce the session. These files are in
ASCII format and can be edited or written in a text editor. For details, see New Session Command (p. 51).
CCL Files (.ccl)
CFX CCL files are used by CFX-Pre to save CFX Command Language (CCL) statements. CCL files differ
from session files in that only a snapshot of the current state is saved to a file. These files are in ASCII
format and can be edited or written in a text editor. The CCL statements stored in these files replace or
append the existing CCL data, depending on the option chosen. For details, see:
•
Import CCL Command (p. 35)
•
Append or Replace (p. 35).
An overview of the files used throughout ANSYS CFX is available in ANSYS CFX File Types in the CFX
Introduction.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
15
16
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 2: CFX-Pre 3D Viewer
In CFX-Pre, the 3D viewer is visible whenever a partial or complete case is loaded. After importing a
mesh into CFX-Pre, you can see a visual representation of the geometry in the 3D viewer. You can create
various other objects that can be viewed in the 3D viewer; for details, see "CFD-Post Insert Menu". The
visibility of each object can be turned on and off using the check boxes in the tree view; for details,
see Object Visibility (p. 18).
Descriptions of the various viewing modes and 3D viewer commands, including toolbars, shortcut
menus, and hotkeys, are given in 3D Viewer Modes and Commands (p. 19).
You can switch between four adjustable “views” that each remember the camera angle and state of
visibility of all objects.
The 3D viewer can display multiple viewports at a time. The viewport arrangement is controlled from
the viewer toolbar.
This chapter describes:
2.1. Object Visibility
2.2. 3D Viewer Modes and Commands
2.3. Views and Figures
2.4. Stereo Viewer
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
17
Chapter 2: CFX-Pre 3D Viewer
Note
In order to see correct colors and accurately displayed objects in the 3D Viewer, some combinations of ATI video cards and ATI graphics drivers on Windows XP require that you set
the environment variable VIEWER_CACHE_COLORS to 0:
1.
Right-click on My Computer and select Properties. The System Properties dialog box
appears.
2.
Click the Advanced tab.
3.
Click Environment Variables.
4.
Under System variables, click New.
5.
In the Variable name field, type: VIEWER_CACHE_COLORS
6.
In the Variable value field, type the number: 0
7.
Click OK.
8.
To verify the setting, open a command window and enter: set
The results should include the line:
VIEWER_CACHE_COLORS=0
This setting will fix problems such as:
•
Boundary condition markers placed incorrectly or rendered in white.
•
Regions around the circles are incorrect (rendered as yellow areas marked with blue)
•
Mesh lines not displayed properly and with dark patches showing.
2.1. Object Visibility
The visibility of each object can be turned on and off using the check boxes in the tree view, as described
in Object Visibility. However, you can also hide objects by right-clicking on them and selecting Hide.
The shortcut menu has a title that indicates the object that will be acted upon so that you do not accidentally hide the wrong object. In the figure that follows, the user right-clicked on an object named
Primitive 2D A.
18
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3D Viewer Modes and Commands
Once an object has been hidden, you can show it again by selecting that object's check box in the
Outline view.
2.2. 3D Viewer Modes and Commands
The topics in this section include:
•
3D Viewer Toolbar (p. 19)
•
Shortcut Menus (p. 21)
•
Viewer Hotkeys (p. 23)
•
Mouse Button Mapping (p. 24)
•
Picking Mode (p. 26)
•
Boundary Markers and Labels (p. 27)
2.2.1. 3D Viewer Toolbar
The 3D Viewer toolbar has the following tools:
Tool
Description
Makes one of the picking tools active.
Selects objects.When a number of objects overlap, the one closest
to the camera is picked. In CFX-Pre, when selecting regions for
boundaries, if more than one region is under the mouse pointer
at the location that you click, those regions will be listed in a list
box, allowing you to select the intended region.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
19
Chapter 2: CFX-Pre 3D Viewer
Tool
Description
Selects objects using a box. Drag a box around the objects you
want to select.
Selects objects using an enclosed polygon. Click to drop points
around the objects. Double-click to complete the selection.
Note
Polygon Select mode will not allow you to create
an invalid region, such as would occur if you attempted to move a point such that the resulting
line would cross an existing line in the polygon.
When you select Insert > Primitive Region, the paint can icon
causes the all the mesh elements on the selected face (that are not
currently part of a primitive region) to be selected for a new primitive region.The “counter” widget enables you to change the crease
angle in degrees used to decide where the flood-pick algorithm
will stop.
When you select Insert > Primitive Region, this feature controls
which objects you can select.
Select Visible Only treats the contents of the Viewer as
opaque and enables you to select only the top mesh elements at any point.
Select Any Depth treats the contents of the Viewer as
“transparent” and enables you to select any of the mesh
elements that you would encounter if you drilled through
the object at a given point. You use this option with the
depth indicator in the bottom-left of the Viewer.
When you select Insert > Primitive Region, this feature controls
which mesh elements you can select with a box or enclosed polygon.
Choose Fully Enclosed selects only the mesh elements
that have boundaries that are completely within the box
or polygon you draw.
Choose Enclosed and Touching selects both the mesh
elements that are completely within the box or polygon
you draw as well as any mesh elements of which any part
is within that area.
These icons allow primitives to be chosen over composites or vice
versa.This feature is selected only when you are in the single-select
picking mode.
Rotates the view as you drag with the mouse. Alternatively, hold
down the middle mouse button to rotate the view.
20
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3D Viewer Modes and Commands
Tool
Description
Pans the view as you drag with the mouse. Alternatively, you can
pan the view by holding down Ctrl and the middle mouse button.
Adjusts the zoom level as you drag with the mouse vertically. Alternatively, you can zoom the view by holding down Shift and the
middle mouse button.
Zooms to the area enclosed in a box that you create by dragging
with the mouse. Alternatively, you can drag and zoom the view by
holding down the right mouse button.
Centers all visible objects in the viewer.
Toggles highlighting according to the highlighting preferences
(select Edit > Options > CFX-Pre > Object Highlighting > Type).
Highlighting is active only when the viewer is set to Picking Mode.
For details, see Picking Mode.
Enables you to select mesh nodes.When picking a point from the
viewer to populate a widget that defines a coordinate, the point
can either be a point in space or a mesh “node”.This tool enables
you to select the mesh node nearest to the location you click.
Displays the Labels and Markers dialog box that is used to select/clear the display of named regions and markers in the viewer.
For details, see Boundary Markers and Labels.
Selects the viewport arrangement.You can perform Independent
zoom, rotation and translate options in each viewport.
Toggles between locking and unlocking the views of all viewports.
When the views are locked, the camera orientation and zoom level
of the non-selected viewports are continuously synchronized with
the selected viewport. Locking the view for the viewports in this
way can be a useful technique for comparing different sets of visible
objects between the viewports.This tool is available only when all
viewports are using the Cartesian (X-Y-Z) transformation.
Displays the Viewer Key Mapping dialog box. See Viewer Hotkeys
for details.
2.2.2. Shortcut Menus
You can access the shortcut menu by right-clicking anywhere on the viewer. The shortcut menu is different depending on where you right-click.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
21
Chapter 2: CFX-Pre 3D Viewer
2.2.2.1. CFX-Pre 3D Viewer Shortcut Menu
2.2.2.1.1. Shortcuts for CFX-Pre (Viewer Background)
The following commands are available in CFX-Pre when you right-click the viewer background:
Command
Description
Import Library Data
Opens the Select Library Data to Import dialog box so that you can add a new material to the simulation. Examples of such materials include Methanol CH4O, Rubber, Water at 25 C, and many more.
This option is the same as right-clicking on Materials in the tree view and
selecting Import Library Data.
Start Solver
•
Define Run writes the CFX-Solver input file and starts the CFX-Solver Manager.
•
Run Solver writes the CFX-Solver input file and starts the CFX-Solver.
•
Run Solver and Monitor writes the CFX-Solver input file and starts both the
CFX-Solver and the CFX-Solver Manager.
View in CFD-Post
Writes the CFX-Solver input file and start CFD-Post
Write Solver Input
File
The same as selecting Tools > Solve > Write Solver Input File. For details, see Write
Solver Input File Command.
Create New View ...
Creates a new view.The new view will become the current view. For more information
about views, see Views and Figures.
Delete View
Delete the current view.
Predefined Camera
Displays different views by changing the camera angle to a preset direc-
tion.
Fit View
Centers all visible objects in the viewer.This is equivalent to clicking the
icon.
Projection
Switches between perspective and orthographic camera angles.
Default Legend
Shows or hides the default legend object.
Axis
Shows or hides the axis orientation indicator (triad) in the bottom-right corner of the
viewer.
Ruler
Shows or hides the ruler on the bottom of the viewer.
Labels
Controls the display of labels. For more information, see Boundary Markers and Labels.
Markers
Controls the display and properties of boundary markers. For more information, see
Boundary Markers and Labels.
22
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3D Viewer Modes and Commands
Command
Description
Save Picture
Same as selecting File > Save Picture. For details, see Save Picture Command.
Viewer Options
Opens the Options dialog box with the viewer options displayed. For details, see
Graphics Style.
2.2.2.1.2. Shortcuts for CFX-Pre (Viewer Object)
The following commands are available in CFX-Pre when you right-click an object in the viewer:
Command
Description
Edit, Edit Definition,
Edit Mesh
Opens the details view for the selected object so that you can edit its properties.
Mesh Statistics
Shows basic information about mesh regions including node count and maximum
element edge length ratio.This command is also available by right-clicking a region
selection in the tree view. For details, see Mesh Statistics.
Insert
Enables you to insert a boundary, interface, subdomain, or source point. For details,
see Boundary Conditions, Domain Interfaces, Subdomains, or Source Points.
Edit in Command Editor
Opens the Command Editor dialog box, displaying the CEL for the selected object.
For details, see Using the Command Editor.
Render
Displays the following render options:
Color enables you to choose a color for the selected object.
Lines enables you to select to Show Wireframe, Show Mesh or No Lines.
Transparency enables you to set the transparency levels of the domain. The
choices are Opaque, 0.25, 0.5, 0.75, or Fully Transparent.
Properties invokes the Render Options dialog box. For details, see Render
Options (p. 88).
Show
Shows the object in the viewer.
Hide
Hides the selected object in the 3D viewer.
Delete
Deletes the selected object.
Rename
Changes the selected object’s name.
Alternatives
When you right-click a location in the viewer, CFX-Pre presents a shortcut menu for
one object at that location. Shortcut menus for the other objects at the same location
are accessible as submenus under the Alternatives heading.
2.2.3. Viewer Hotkeys
A number of shortcut keys are available to carry out common viewer tasks. These can be carried out
by clicking in the viewer window and pressing the associated key.
Key
Action
space
Toggles between picking and viewing mode.
arrow keys
Rotates about horizontal and vertical axes.
Ctrl + up/down arrow keys
Rotates about an axis normal to the screen.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
23
Chapter 2: CFX-Pre 3D Viewer
Key
Action
Shift + arrow keys
Moves the light source.
1
Switches to one viewport.
2
Switches to two viewports.
3
Switches to three viewports.
4
Switches to four viewports.
c
Centers the graphic object in the viewer window.
n
Toggles the projection between orthographic
and perspective.
r
Resets the view to the initial orientation.
s
Toggles the level of detail between auto, off, and
on.
u
Undoes transformation.
Shift-u
Redoes transformation.
x
Sets view from +X axis.
Shift-x
Sets view from -X axis.
y
Sets view from +Y axis.
Shift-y
Sets view from -Y axis.
z
Sets view from +Z axis.
Shift-z
Sets view from -Z axis.
The information in this table is accessible by clicking the Show Help Dialog
viewer toolbar.
toolbar icon in the 3D
2.2.4. Mouse Button Mapping
The mouse mapping options enable you to assign viewer actions to mouse clicks and keyboard/mouse
combined clicks. To adjust or view the mouse mapping options, select Edit > Options, then Viewer
Setup > Mouse Mapping.
24
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3D Viewer Modes and Commands
Figure 2.1 Mouse Mapping using Workbench Defaults
Table 2.1 Mouse Operations and Shortcuts
Operation
Description
Workbench Mode
Shortcuts
CFX Mode Shortcuts
Zoom
To zoom out, drag the pointer up; to
zoom in, drag the pointer down.
Shift + middle mouse
button
Middle mouse
button
Object
Zoom
Shift + middle
mouse button
zooms in a step.
Camera
Zoom
Shift + right
mouse button
zooms out a
step.
Translate
Drag the object across the viewer.
Ctrl + middle mouse
button
Right mouse button
Zoom Box
Draw a rectangle around the area of
interest, starting from one corner and
ending at the opposite corner. The selected area fills the viewer when the
mouse button is released.
Right mouse button
Shift + left mouse
button
Shift + left
mouse button
Shift + right
mouse button
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
25
Chapter 2: CFX-Pre 3D Viewer
Operation
Description
Workbench Mode
Shortcuts
CFX Mode Shortcuts
Rotate
Rotate the view about the pivot point Middle mouse button
(if no pivot point is visible, the rotation
point will be the center of the object).
Set Pivot
Point
Set the point about which the Rotate
actions pivot. The point selected must
be on an object in the 3D Viewer.
When you set the pivot point, it appears as a small red sphere that moves
(along with the point on the image
where you clicked) to the center of the
3D Viewer. To hide the red dot that
represents the pivot point, click on a
blank area in the 3D Viewer.
Left mouse button
when in rotate, pan,
zoom, or zoom box
mode (as set by the
icons in the viewer's
tool bar).
Ctrl + middle mouse
button
Move Light
Move the lighting angle for the 3D
Viewer. Drag the mouse left or right
to move the horizontal lighting source
and up or down to move the vertical
lighting source. The light angle hold
two angular values between 0 - 180.
Ctrl + right mouse
button
Ctrl + right mouse
button
Picking Mode
Select an object in the viewer.
Ctrl + Shift + left
mouse button
Ctrl + Shift + left
mouse button
2.2.5. Picking Mode
Picking mode is used to select and drag objects in the viewer. The mesh faces must be visible on an
object or region to allow it to be picked. Enter picking mode by selecting the Single Select
a pull-down menu of the viewer toolbar. If the Single Select
click the New Selection
tool in
icon is already visible, you can simply
icon.
You can also pick objects while still in viewing mode by holding down the Ctrl and Shift keys as you
click in the viewer.
2.2.5.1. Selecting Objects
Use the mouse to select objects (for example, points and boundaries) from the viewer. When a number
of objects overlap, the one closest to the camera is picked.
You can change the picking mode by selecting one of the toolbar icons:
•
Single Select
•
Box Select
•
Polygon Select
For details on the operation of the toolbar icons, see 3D Viewer Toolbar (p. 19).
26
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Views and Figures
2.2.6. Boundary Markers and Labels
Click Case Options > Labels and Markers to invoke the Labels and Markers Options details
view, used to select/clear the display of named regions and markers in the viewer as well as change
the appearance of the markers.
Also see Boundary Condition Visualization (p. 164) for more details.
2.2.6.1. Label Options
Select the options to enable label visibility. To disable all labels, clear the Show Labels option. The first
three options refer to primitive and composite regions. For details, see Assemblies, Primitive Regions,
and Composite Regions (p. 91).
2.2.6.2. Boundary Markers
The Show Boundary Markers option turns on boundary condition symbols such as arrows indicating
flow direction at an inlet.
The Marker Quantity slider controls the number of markers displayed. Moving the slider to the right
increases the number.
The Marker Length slider controls the size of the markers displayed. Moving the slider to the right increases the size.
2.2.6.3. Boundary Vectors
The Vector Quantity slider controls the number of vectors displayed. Moving the slider to the right
increases the number.
The Vector Length slider controls the size of the vectors displayed. Moving the slider to the right increases the size.
See Boundary Plot Options Tab (p. 163) for a discussion of displaying boundary vectors.
2.3. Views and Figures
The 3D Viewer opens with a single viewport; you can increase the number of viewports to four by using
the viewport icon:
Figure 2.2 Viewport Control
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
27
Chapter 2: CFX-Pre 3D Viewer
The contents of a viewport are a view, which is a CCL object that contains the camera angle, zoom level,
lighting, and visibility setting of each object in the tree view.
Each viewport contains a different, independent view. By default, four views exist: View 1, View 2, View
3, View 4.
When you select an object in the tree view, its information is applied to the active viewport. When you
manipulate an object in the viewport, the view's CCL is updated immediately. However if the focus is
on that viewport, you can press u to revert your change.
2.3.1. Switching to a View or Figure
To switch to a view or figure, do one of the following:
•
Use the drop-down menu in the upper-left corner of the viewport.
•
For figures only: Double-click the figure in the tree view (under the Report object).
•
For figures only: Right-click the figure in the tree view (under the Report object), then select Edit from
the shortcut menu.
2.3.2. Changing the Definition of a View or Figure
To change a view or figure:
1.
Switch to the view or figure that you want to change.
For details, see Switching to a View or Figure (p. 28).
2.
Change the view or figure (for example, rotate the view).
View and figure objects are saved automatically when you switch to a different view or figure.
2.4. Stereo Viewer
If you:
1.
Have a standard stereo display
2.
Have a graphics card that supports quad buffering OpenGL output
3.
Have set your graphics card to "Stereo"
4.
Have set your view to Perspective mode (right-click in the Viewer and select Projection > Perspective)
...you can view output in stereo1. To enable this functionality:
1.
Select Edit > Options.
2.
In the Options dialog box, select CFX-Pre > Viewer.
3.
On the Viewer panel:
a.
1
Set the Stereo Mode to Stereo.
The stereo viewer feature has been tested on:
•
XP-64 and Vista-64 with an NVidia graphics card and a Planar Stereo Monitor
•
XP-64 with an ATI card and a Zalman Stereo Monitor.
28
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Stereo Viewer
b.
4.
Set the Stereo Effect. The value of the "stereo effect" that is required is related to the distance
between the observer and the display. If the stereo effect is too strong, either move away from
the display, or move the slider towards Weaker.
Click OK to save the settings.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
29
30
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 3: CFX-Pre File Menu
There are a number of basic functions available in CFX-Pre, such as opening and saving an existing
case. These are described in detail in this chapter:
3.1. New Case Command
3.2. Open Case Command
3.3. Close Command
3.4. Save Case Command
3.5. Save Project Command
3.6. Refresh Command (ANSYS Workbench only)
3.7. Save Case As Command
3.8. Import Mesh Command
3.9. Reload Mesh Files Command
3.10. Import CCL Command
3.11. Export CCL Command
3.12. Save Picture Command
3.13. Recent Case Files Submenu
3.14. Recent CCL Files Submenu
3.15. Recent Session Files Submenu
3.16. Quit Command
3.1. New Case Command
Note
If a case is open, New Case is not available. To create new cases, ensure all open cases are
saved (if required) and closed.
1.
Select File > New Case.
The New Case dialog box appears.
2.
Select a case type.
•
General makes use of all features in CFX-Pre. This is the most common mode of operation.
•
Turbomachinery is used specifically for turbomachinery applications and enables quick setup in
such cases. For details, see Turbomachinery Mode (p. 323).
•
Quick Setup provides fewer model options and is suitable for simple physics setup. It is useful as
a tool to learn the basic paradigms of CFX-Pre before using General mode. For details, see Quick
Setup Mode (p. 319).
•
Library Template enables a CCL physics definition to be imported for use on a mesh. For details,
see Library Objects (p. 331).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
31
Chapter 3: CFX-Pre File Menu
3.2. Open Case Command
The Open Case command can be used to open existing CFX-Pre case files (.cfx), as well as implicitly
start a new case by opening a *.def, *.mdef, *.res, .ccl, “full” transient results file (*.trn), or
backup file (*.bak). Other supported file types include: Mesh or Simulation Database file (*.cmdb or
*.dsdb), and GTM Database file (.gtm).
Note
If a case is already open, Open Case is not available. To open cases, ensure that all open
cases are saved (if required) and closed.
1.
Select File > Open Case.
The Load Case File dialog box appears.
2.
Select a location to open the file from.
3.
Under Files of type, select the type of file to open.
4.
•
Case files can be selected. CFX case files (*.cfx) contain all of the physics, region, and mesh information for your case. For details, see Opening Case (.cfx) Files (p. 33).
•
CFX-Solver input or result files can be selected. For details, see Opening CFX-Solver Input (.def, .mdef),
Results (.res), Transient (.trn) or Backup (.bak) Files (p. 33).
•
CCL files can be selected. For details, see Opening CCL (.ccl) Files (p. 33).
•
Mesh or Simulation Database files can be selected. For details, see Opening Meshing (.cmdb or .dsdb)
Files (p. 33).
•
GTM Database files can be selected. For details, see Opening CFX-Mesh (.gtm) Files (p. 34).
Select the file to open and click Open.
Note
When CFX-Solver input or results files from a previous release of CFX are opened in CFX-Pre,
physics errors are highlighted in red in the message area. If these errors are ignored, a case
can still run in the CFX-Solver in many cases, but it is recommend that the errors be fixed.
This ensures CCL is updated to the current version. These errors are usually fixed easily by
right-clicking on the object and selecting Auto Fix Physics. Also, double-clicking on the error
in the message area opens the details view in which the error was made. For details, see
Physics Errors from Old .def/.res Files (p. 12). Also, the Command Editor can be used to correct
CCL. For details, see Command Editor Dialog Box (p. 335).
3.2.1. Recover Original Session
When opening a CFX-Solver input file, the option Recover Original Session can be used to find the
location of the original CFX Case file (that was used to generate the CFX-Solver input file) and load it.
Using this option enables CFX-Pre to access more information (such as composite regions, unused materials and meshes, layouts, and views) and then write that information to the CFX-Solver input file.
32
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Open Case Command
When the Recover Original Session option is selected, the Replace Flow Data option is available. This
will extract the CCL from the CFX-Solver input file and replace the existing Case file data. This is useful
to recover the problem definition when it has been modified outside of CFX-Pre during the run.
3.2.2. Opening Case (.cfx) Files
When opening an existing case file, CFX-Pre opens the case in the state in which it was last saved, including the mesh.
3.2.3. Opening CFX-Solver Input (.def, .mdef), Results (.res), Transient (.trn)
or Backup (.bak) Files
CFX-Solver input and results files from the current and previous releases of CFX can be opened. When
opening these files, a new case file is created. The mesh and physics are imported into the new case.
All pre-processing information in these files is imported into CFX-Pre and is edited in the same way as
in other case files.
CFX-Pre can also load “full” transient results file (*.trn) or backup file (*.bak) by typing *trn or
*bak, respectively, as the File Name in the Load Case File dialog box. Using the * character returns
a list of available files of type *.trn or *.bak. The selected file is imported as a CFX-Solver input file.
Note
•
If a Release 11.0 .def file containing automatically generated interfaces is loaded into CFXPre, and these interfaces were generated as a result of 'contact' information in the original
.cmdb file, these interfaces may be removed by CFX-Pre. This is a problem only when loading
Release 11.0 .def files, and will occur only in a small percentage of cases. Loading a .cfx
file will work correctly.
•
It is not possible to load an .mres file into CFX-Pre.
3.2.4. Opening CCL (.ccl) Files
Opening a CCL file creates a new case file. Any physics, material and expression information is imported
into CFX-Pre and can be edited in the same way as for case files. CCL files do not contain any mesh
data, so it is necessary to import a mesh before assigning locations to domains and boundary conditions.
3.2.5. Opening Meshing (.cmdb or .dsdb) Files
Opening a .cmdb or .dsdb file loads the mesh and creates an initial physics state, in the same manner
as creating a new case.
Important
.cmdb and .dsdb files require the cfxacmo library, which is supplied with ANSYS Workbench.
If you are unable to load such files into CFX-Pre, one solution is to install ANSYS Workbench
to make those library files available.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
33
Chapter 3: CFX-Pre File Menu
3.2.6. Opening CFX-Mesh (.gtm) Files
Opening a .gtm file loads the mesh and creates an initial physics state, in the same manner as creating
a new case.
3.3. Close Command
Closes the existing case, prompting to save if appropriate.
3.4. Save Case Command
When CFX-Pre is started from the ANSYS CFX Launcher, the Save Case command writes the current
state to the case file. You should save a case before closing it to be able to reopen it at a later date; all
data is lost if CFX-Pre is closed without saving the case.
When CFX-Pre is started from ANSYS Workbench, the Save Project command writes the current state
of the project.
3.5. Save Project Command
When CFX-Pre is started from ANSYS Workbench, the Save Project command writes the current state
of the project.
3.6. Refresh Command (ANSYS Workbench only)
Reads the upstream data, but does not perform any long-running operation.
3.7. Save Case As Command
When using Save As, the previous case files are closed and remain unchanged from the last time they
were explicitly saved.
1.
Select File > Save Case As.
The Save Case dialog box appears.
2.
Select a location where the file will be saved.
3.
Under File name, type the name to save the file as.
4.
Click Save.
A new file is saved and is kept open in CFX-Pre.
3.8. Import Mesh Command
Numerous options are available when importing a mesh. For details, see Importing Meshes (p. 65).
3.9. Reload Mesh Files Command
It is possible to import and manipulate many meshes within a CFX-Pre case. In some cases, this can
result in a complex set of operations (for example, a single 'blade' mesh may have been imported, and
then 30 copies may have been made). In some cases, it is desirable to swap this mesh for one that is
much finer, or of better quality. The process of deleting all existing meshes, re-importing the new mesh
34
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Import CCL Command
and then applying the transformations again could be costly. Hence, the mesh reload function enables
one or more mesh files to be replaced in a fraction of the time.
1.
Select File > Reload Mesh Files.
The Reload Mesh Files dialog box appears.
2.
Select or clear the mesh files to replace the ones that were previously imported.
3.
Click OK.
Note
This feature is not required (and is not available) in CFX-Pre launched from ANSYS Workbench.
3.10. Import CCL Command
CFX Command Language (CCL) consists of commands used to carry out actions in CFX-Pre, the CFXSolver Manager and CFD-Post. All of the steps carried out in CFX-Pre are executed as CCL commands
in the software’s engine, and these commands can be exported and imported to other cases.
Tip
•
You can also import expressions and regions using the Import CCL command.
•
To import composite region definitions from older versions of CCL, use the Import CCL
command found in the File menu, rather than the import command found in the Regions
workspace.
A useful application of importing CCL is to apply the same pre-processing data to a number of different
meshes. In such a case, the following general workflow may be ensued:
1.
Import the new mesh.
2.
Import the CCL data.
3.
Assign mesh locations to the domains and boundary conditions, if required.
4.
Write the CFX-Solver input file for the CFX-Solver.
The benefit of using this workflow is that there would be no need to specify all of the pre-processing
data again.
Importing a set of commonly used customized material or reaction definitions is also possible by importing a CCL file. A useful application of the import CCL feature is demonstrated when using Library
Mode. For details, see Library Objects (p. 331).
3.10.1. Append or Replace
3.10.1.1. Append
This option never deletes existing objects such as domains, boundary conditions, initialization, and so
on. Objects with a different name than existing objects are added. If an object of the same name and
type already exists, parameters within the object that are unique to the imported CCL file are added to
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
35
Chapter 3: CFX-Pre File Menu
the existing object. When the imported CCL file contains parameter definitions that already exist within
existing objects, they will replace the existing definitions.
3.10.1.2. Replace
This option overwrites, in full, existing objects of the same name and type. Because boundary conditions,
subdomains, and so on are defined within a domain, if that domain is replaced, these objects are lost
if not defined in the imported CCL file. Objects with a unique name are added to the existing case.
3.10.1.2.1. Auto-load materials
When Replace is selected, the Auto-load materials check box is made available. When a file is imported
with the Auto-load materials check box selected, any materials and reactions that are missing from
the problem setup being imported, and that are not defined in the case already, will be loaded automatically. These added materials and reactions can be found in the standard materials and reactions
library files.
3.11. Export CCL Command
Using Export CCL, some or all CCL definitions can be exported to a file.
1.
Select File > Export > CCL.
The Export CCL dialog box appears.
2.
Select or clear Save All Objects.
A list of all existing CCL objects is available. To export particular objects, clear Save All Objects
and select only the objects to export. For details, see Save All Objects (p. 36).
3.
Select a location to export to.
4.
Enter a name for the exported file.
5.
Click Save.
To export the physics definition for a problem, select all the FLOW objects. Additional Variables, CEL
expressions, User Functions and material definitions are stored in LIBRARY objects; these will need to
be included if you want to export these objects.
3.11.1. Save All Objects
When Save All Objects is selected, all CCL object definitions are written to the CCL file. To export only
a sub-set of CCL objects, clear this and select only the required CCL objects.
3.11.1.1. Sample of Saving CEL Expressions
This sample is specifically for the export of expressions.
1.
Select File > Export > CCL.
2.
Clear Save All Objects and expand LIBRARY.
3.
Expand CEL.
4.
Select EXPRESSIONS.
5.
Select a location to export to.
36
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Save Picture Command
6.
Enter a name for the exported file.
7.
Click Save.
3.12. Save Picture Command
The current contents of the viewer can be saved to a file.
1.
Select File > Save Picture.
The Save Picture dialog box appears.
2.
Enter a name for the file. You may enter the file name and path into the File text box, or click the
Browse
3.
icon and search for the directory in which the file is to be saved.
If you have used the Browse
feature, click Save.
The Save Picture dialog box displays the path and name of the file. If a new format was selected,
the default extension changes on this dialog box as well.
4.
Under Format, select the output style of the image.
•
Portable Network Graphics (*.png) is a file format intended to replace the GIF format. It was designed for use on the World Wide Web and retains many of the features of GIF with new features
added.
•
CFD Viewer State (3D) is a 3D file format that can be read back directly into a stand-alone
CFD Viewer.
•
JPEG (*.jpg) is a compressed file format developed for compressing raw digital information. File
sizes are small but it is not recommended for line drawings.
•
Bitmap (*.bmp) files are usually large and do not adjust well to resizing or editing. They do retain
all of the quality of the original image and can be easily converted to other formats.
•
Portable Pixel Map (*.ppm) is similar to the Bitmap format.
•
PostScript (*.ps) and Encapsulated PS (*.eps) are generally recommended for output to a
printer or line drawings. However, labels1, the ruler 2 and transparency3 will cause the PS/EPS to
output as a very large bitmap file, in which case a PNG file would be a more efficient alternative.
Note that the ANSYS logo and the axis do not cause the PS/EPS output to become a bitmap.
•
5.
Virtual Reality Modeling Language (VRML, *.wrl) is used to present interactive three-dimensional
views and can be delivered across the World Wide Web. The only supported VRML viewer is Cortona
from Parallel Graphics (see http://www.parallelgraphics.com/products/cortona/).
Select or clear Use Screen Capture.
If selected, a screen capture of the viewer is saved to the output. Note that Face Culling affects
printouts done using screen capture mode only.
6.
Select or clear White Background.
1
You can hide labels from Edit > Options > CFX-Pre > Labels and Markers > Labels.
2
You can hide the ruler from Edit > Options > CFX-Pre > Graphics Style > Visibility > Ruler Visibility.
3
You can control transparency from Edit > Render > Transparency.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
37
Chapter 3: CFX-Pre File Menu
If selected, white objects appear in black and black objects appear in white in the image file (except
VRML). All objects are affected by this toggle and slightly off-white and off-black objects are also
inverted.
7.
Select or clear Enhanced Output (Smooth Edges).
If selected, the image is processed by antialiasing.
8.
Select or clear Use Screen Size.
If selected, the current screen size is used. Otherwise, set a width and height.
9.
Select or clear Scale (%).
If selected, the size of the image is reduced or increased to a percentage of the current viewer
screen size.
10. If exporting to JPEG format, select or clear Image Quality.
Set between 0 (lowest) and 100 (highest).
11. Set a Tolerance.
The default tolerance is 0.0001. This is a non-dimensional tolerance used in face sorting when
generating hardcopy output. Larger values result in faster printing times, but may cause defects
in the resulting output.
Note that the paper orientation for printing, portrait or landscape, is determined by the size of the
viewer window. If the height of the window is larger then the width, then portrait is used. If the width
is larger then the height, then landscape is used.
Important
When a clip plane is coincident with regions, boundaries, or interfaces that are planes, the
results of a Save Picture command may not match what you see in the 3D Viewer (depending
on the orientation of the case). In this situation, select the Use Screen Capture check box.
3.13. Recent Case Files Submenu
CFX-Pre saves the file paths of the last five case files (.cfx) opened. To open one of these case files,
select File > Recent Case Files.
3.14. Recent CCL Files Submenu
CFX-Pre saves the file paths of the last five CCL files opened. To open one of these CCL files, select File
> Recent CCL Files.
3.15. Recent Session Files Submenu
CFX-Pre saves the file paths of the last five session files opened. To open one of these session files
(*.pre), select File > Recent Session Files.
38
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quit Command
3.16. Quit Command
To quit CFX-Pre, select File > Quit. In stand-alone mode, if the case is not already saved, there will be
a prompt as to whether a save should be done.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
39
40
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 4: CFX-Pre Edit Menu
This chapter describes:
4.1. Undo and Redo
4.2. Options
Undo and Redo commands are available in the Edit menu. Additionally, there are a variety of options
that can be set to customize the software.
4.1. Undo and Redo
The undo and redo capability is limited by the amount of available memory.
In stand-alone mode, the undo stack is cleared whenever a New, Open, or Close action occurs. Similarly,
when using CFX-Pre/CFD-Post from within ANSYS Workbench, the undo stack is cleared in CFX-Pre/CFDPost after the application receives commands from ANSYS Workbench.
Issue the Undo command by doing any of the following:
•
Select Edit > Undo.
•
Click Undo
•
Press Ctrl + Z
on the toolbar.
Note
•
You can repeatedly issue the Undo command.
•
Some viewer manipulations cannot be reverted using the Undo command.
•
Some commands that you issue have multiple components. For example, when you create
some objects the software creates the object and sets the visibility of the object on (in two
separate operations). Thus, when you perform an undo operation in such a situation, you
are setting the visibility of the object off; you must choose undo a second time to “uncreate”
the object.
•
Undo cannot be used when recording session files.
The redo feature is used to do an action that you have just undone using the Undo command. Issue
the Redo command by doing any of the following:
•
Select Edit > Redo.
•
Click Redo
•
Press Ctrl + Y
on the toolbar.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
41
Chapter 4: CFX-Pre Edit Menu
4.2. Options
The Options dialog box enables you to set various general preferences. Settings are retained per user.
1.
Select Edit > Options.
The Options dialog box appears.
2.
Set options as required. For descriptions of the available options, see:
•
CFX-Pre Options (p. 42)
•
Common Options (p. 47)
If desired, you can use the CFX Defaults or the Workbench Defaults buttons at the bottom of
the dialog box to quickly set CFX-Pre, CFX-Solver Manager, and CFD-Post to have the standard
appearance and operation of CFX or Workbench respectively. The only CFX-Pre settings that are
affected by these buttons are:
3.
•
CFX-Pre > Graphics Style > Background > Color Type
•
CFX-Pre > Graphics Style > Background > Color
•
CFX-Pre > Colors > Labels
•
CFX-Pre > Colors > Legend Text
•
CFX-Pre > Colors > Turbo Axis
•
Common > Viewer Setup > Mouse Mapping
Click OK.
Note
Changes made under the Options dialog box do not take effect until a new case is opened.
When changing some user preferences, it will be necessary to restart the application for the
setting to take effect. For example, changes to the highlighting mode, whether made in the
Edit > Options panel or from the Outline tree Case Options > General > General Options
panel, do not take place until the application is restarted.
4.2.1. CFX-Pre Options
When the Options dialog box appears, the CFX-Pre options can be configured under CFX-Pre.
•
Record Default Session File
When selected, a session file named cfx.xx.pre will be recorded automatically each time CFXPre is started (where 'xx' is the next available number). For more information on session files, see
Playing a Tutorial Session File.
•
Default User Mode can be set to General, Turbo, or Quick Setup.
This determines the default mode that CFX-Pre will use when creating a simulation. For details on
Turbo mode, see Turbomachinery Mode (p. 323). For details on Quick Setup mode, see Quick Setup
Mode (p. 319).
42
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Options
•
Report CCL Update Summary produces an information window when you load a file that contains
CCL from a previous version of CFX-Pre. This window describes the updates that were made to the CCL
to make it compatible with the current software release.
4.2.1.1. General
Settings made here set the default operation for CFX-Pre; however, you can override these settings for
your current simulation by going to the Outline tree view and editing Case Options > General.
4.2.1.1.1. Auto Generation
•
Automatic Default Domain
When this option is selected, a domain with the name Default Domain will be created upon
importing a mesh.
To toggle default domain generation on or off for a session, without affecting the user preference
setting, you can right-click the Simulation object in the tree view and select Automatic Default
Domain from the shortcut menu.
If you manually delete a default domain, the default domain mechanism will be disabled, and a
warning message will appear in the physics message window.
If you create a domain that uses the same region(s) as the default domain, the latter will be redefined
with the remaining locations, or deleted if all the regions are referenced by user-defined domains.
If you modify the location of the default domain, the name will change to Default Domain
Modified and no additional default domain will be generated.
When loading an existing case (cfx file or def file), if there are any mesh volumes that are not
assigned to a domain, the default domain generation will be disabled. It can be re-activated as
described previously.
•
Automatic Default Interfaces
When selected, CFX-Pre will attempt to create domain interfaces when a domain is created or
modified.
To toggle default interface generation on or off for a session, without affecting the user preference
setting, you can right-click the Simulation object in the tree view and select Automatic Default
Interfaces from the shortcut menu.
Domain interface generation is always deactivated when loading an existing simulation.
•
Interface Method
When Automatic Default Interfaces has been selected, the Interface Method can be set to one
of the following to control how interfaces are automatically generated between domains where
regions are found to be connected:
–
One per Interface Type
This method groups as many domains into as few interfaces as possible.
–
One per Domain Pair
An interface is generated for each pair of domains.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
43
Chapter 4: CFX-Pre Edit Menu
•
Default Boundary can be set to one of the following:
–
Standard
A default boundary condition is created that covers all primitive regions that are not assigned
to any boundary condition in the current domain. The default boundary is modified dynamically
when other boundary conditions are subsequently added or deleted such that it includes all
regions not assigned to any other boundary condition.
–
One per Relevant Region
A default boundary condition on each relevant region not assigned to any boundary condition
is created. In this context, ‘relevant’ means every composite 2D region, plus any 2D primitive
regions that are not referenced by a composite 2D region. If boundary conditions are subsequently deleted, causing some regions to be unassigned, a single default boundary condition
will include all such regions.
–
One per Primitive Region
A default boundary condition on each individual 2D primitive region not assigned to any
boundary condition is created. If boundary conditions are subsequently deleted, causing some
regions to be unassigned, a single default boundary condition will include all such regions.
–
Disabled
4.2.1.1.2. Physics
•
Disable Physics Validation
This option prevents CFX-Pre from issuing messages in the physics message window. For details,
see Physics Message Window (p. 11).
•
Enable Beta Features
Some beta features are hidden in the user interface. You can select this option to unhide those
beta features. When selected, such Beta features will be identified by "(Beta)" in the user interface.
•
Automatic Physics Update
If this option is selected and you change settings in the simulation definition, CFX-Pre will, for
certain settings, respond by changing other settings automatically in an attempt to make problem
specification consistent. This incurs an overhead, so for large problems you may want to disable
this feature.
•
Show Interface Boundaries in Outline Tree
Shows the interface boundaries in the Outline view.
4.2.1.2. Graphics Style
Settings made here set the default operation for CFX-Pre; however, you can override these settings for
your current simulation by going to the Outline tree view and editing Case Options > Graphics Style.
4.2.1.2.1. Object Highlighting
Controls how an object that is generated after a change to the setting of this option is highlighted in
the viewer. Such highlighting occurs when in picking mode, when selecting a region in a list, or when
selecting items in the tree view.
44
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Options
Under Type, select one of the following:
•
Surface Mesh: Displays the surface mesh for selected regions using lines.
•
Face Highlight: Displays the selected regions using faces.
•
Wireframe: Traces objects that contain surfaces with green lines.
•
Bounding Box: Highlights the selected objects with a green box.
Note
When you load a case, the highlighting is dictated by the setting that is stored in the case,
rather than by the current preferences setting.
4.2.1.2.2. Background
Set Mode to Color or Image.
4.2.1.2.2.1. Color
Use Color Type to set either a solid color or a gradient of colors; use Color to set the color (and Color
2 for gradients).
4.2.1.2.2.2. Image
Select one of a list of predefined images or a custom image.
If selecting a custom image, choose an image file and a type of mapping. Image types that are supported
include *.bmp (24-bit BMP only), *.jpg, *.png, and *.ppm. Mapping options are Flat and
Spherical. Flat maps are stationary while spherical maps surround the virtual environment and rotate
with the objects in the viewer.
Custom images have some restrictions: all background images and textures sent to the viewer must be
square and must have dimensions that are powers of 2 (for example, 512 x 512 or 1024 x 1024).
If the dimensions of your background image is not a power of 2, the viewer sizes the image to be a
power of 2 by doing bicubic resampling.
To make the background image square, transparent pixels are added to the smaller dimension to make
it the same as the larger dimension. The transparent pixels enable you to see the regular viewer background, which gives you control over what fill color your background has.
4.2.1.2.3. Colors
4.2.1.2.3.1. Labels
Set the labels to be bright or dark.
4.2.1.2.3.2. Legend Text and Turbo Axis
Select a color by clicking in the box, or clicking the Ellipsis
icon.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
45
Chapter 4: CFX-Pre Edit Menu
4.2.1.2.4. Visibility
4.2.1.2.4.1. Axis and Ruler Visibility
Select or clear Axis Visibility or Ruler Visibility to show or hide the axis indicator or ruler in the
viewer.
4.2.1.3. Render
These settings are used to control the display properties of faces and lines. For details, see Render Options (p. 88).
4.2.1.4. Mesh
Mesh Match Tolerance is used when creating domain interfaces. It is used to determine whether a
one-to-one connection can be made at a domain interface. The tolerance is relative to the local mesh
length scale; the default value is 0.005 (or 0.5%) of the local edge length on the first side of the interface.
A node on the second side must be within this tolerance to a node on the first side for the two to be
considered coincident.
4.2.1.4.1. Mesh Import Options
Source Format specifies which type of mesh file is the general default. For details, see Supported Mesh
File Types (p. 67). Source Directory specifies the default directory from which meshes are imported
upon selecting the Import Mesh command. It is also possible to set other general options (such as
mesh units) and specific advanced options on a per-mesh format basis.
4.2.1.5. Turbo
These settings are used in the recognition of turbo regions when importing a mesh using Turbo mode.
4.2.1.6. Labels and Markers
The settings under this category control whether labels and boundaries appear in the cases displayed
in the 3D Viewer. Settings made here set the default operation for CFX-Pre; however, you can override
these settings for your current simulation by going to the Outline tree view and editing Case Options
> Labels and Markers.
4.2.1.6.1. Labels
The Show Labels option controls whether any labels are displayed; when selected, the remaining options
control whether particular types of labels are displayed.
4.2.1.6.2. Boundary Markers
When Show Boundary Markers is selected, the check boxes in that panel control which markers are
displayed.
The Marker Quantity slider controls the number of markers displayed. Moving the slider to the right
increases the number.
The Marker Length slider controls the size of the markers displayed. Moving the slider to the right increases the size.
46
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Options
4.2.1.6.3. Boundary Vectors
The Vector Quantity slider controls the number of vectors displayed. Moving the slider to the right
increases the number.
The Vector Length slider controls the size of the vectors displayed. Moving the slider to the right increases the size.
See Boundary Plot Options Tab (p. 163) for a discussion of displaying boundary vectors.
4.2.1.7. Extensions
When Include Installed Extension Files is selected, you have the option of creating a comma-separated
list of file to exclude.
4.2.1.8. Customization
The Use Custom Files setting enables the creation of special-purpose interfaces that extend the functionality of CFX-Pre for your environment. Contact your Customer Support representative for more information.
The Force generation of rules files an advanced setting used to maintain synchronization of customized
RULES files. This option is useful during the development of customized RULES files and is available
only when Use Custom Files is selected.
4.2.1.9. Solve
The Definition File Timeout setting controls how long CFX-Pre will wait in seconds while attempting
to obtain enough data from the CFX-Solver in order to spawn a CFX-Solver Manager to monitor an existing batch run. This parameter is used when employing the Simulation Control > Start Solver > Run
Solver and Monitor command to start the CFX-Solver Manager. See Simulation Control in Outline Tree
View Structure (p. 5) for details on monitoring a running solver batch run.
4.2.1.10. Viewer
For details on Stereo settings, see Stereo Viewer (p. 28).
4.2.2. Common Options
Auto Save
Select the time between automatic saves.
To turn off automatic saves, set Auto Save to Never.
Note
This option affects more than one CFX product.
Temporary directory
To set a temporary directory, click Browse
will save state files.
to find a convenient directory where the autosave feature
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
47
Chapter 4: CFX-Pre Edit Menu
4.2.2.1. Appearance
The appearance of the user interface can be controlled from the Appearance options. The default user
interface style will be set to that of your machine. For example, on Windows, the user interface has a
Windows look to it. If, for example, a Motif appearance to the user interface is preferred, select to use
this instead of the Windows style.
1.
Under GUI Style, select the user interface style to use.
2.
For Font and Formatted Font, specify the fonts to use in the application.
Note
It is important not to set the font size too high (over 24 pt. is not recommended) or
the dialog boxes may become difficult to read. Setting the font size too small may
cause some portions of the text to not be visible on monitors set at low resolutions. It
is also important not to set the font to a family such as Webdings, Wingdings, Symbols,
or similar type faces, or the dialog boxes become illegible.
4.2.2.2. Viewer Setup
1.
If you have complicated simulations that feature many overlapping lines, you can specify a Picking
Tolerance that will increase the resolution for picking operations. Values must be between 1 (low
resolution) and 0 (very high resolution); the default value is 0.1. Note that increasing the resolution
will slow printing times.
2.
Select Double Buffering to use two color buffers for improved visualization. For details, see Double
Buffering (p. 48).
3.
Select or clear Unlimited Zoom. For details, see Unlimited Zoom (p. 48).
4.2.2.2.1. Double Buffering
Double Buffering is a feature supported by most OpenGL implementations. It provides two complete
color buffers that swap between each other to animate graphics smoothly. If your implementation of
OpenGL does not support double buffering, you can clear this check box.
4.2.2.2.2. Unlimited Zoom
By default, zoom is restricted to prevent graphics problems related to depth sorting. Selecting Unlimited
Zoom allows an unrestricted zoom.
4.2.2.3. Mouse Mapping
The mouse-mapping options allow you to assign viewer actions to mouse clicks and keyboard/mouse
combinations. These options are available when running in stand-alone mode. To adjust or view the
mouse mapping options, select Edit > Options, then Viewer Setup > Mouse Mapping. For details,
see Mouse Button Mapping.
4.2.2.4. Units
1.
48
Under System, select the unit system to use. Unit systems are sets of quantity types for mass, length,
time, and so on.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Options
The options under System include SI, CGS, English Engineering, British Technical,
US Customary, US Engineering, or Custom. Only Custom enables you to redefine a
quantity type (for example, to use inches for the dimensions in a file that otherwise used SI units).
The most common quantity types appear in the main Options dialog box; to see all quantity
types, click More Units.
2.
Select or clear Always convert units to Preferred Units.
If Always convert units to Preferred Units is selected, the units of entered quantities are immediately converted to those set in this dialog box.
For example, if you have set Velocity to [m s^-1] in this dialog box to make that the preferred
velocity unit, and elsewhere you enter 20 [mile hr^-1] for a velocity quantity, the entered
value is immediately converted and displayed as 8.94078 [m s^-1].
The two sets of units are:
•
The units presented on this dialog box, which control the default units presented in the user interface
as well as the units used for mesh transformation.
•
The solution units. For details, see Setting the Solution Units (p. 197).
4.2.2.4.1. Additional Help on Units
For additional information about units, see Mesh Units (p. 66).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
49
50
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 5: CFX-Pre Session Menu
A session file is a record of the actions performed during a CFX-Pre session, saved in a file as commands.
The actions that cause commands to be written to a session file include:
•
Viewer manipulation performed using the commands available by right-clicking in the viewer window.
•
All actions available from the File and Edit menus.
•
Creation of expressions.
•
Creation of new objects and changes to an object committed by clicking OK or Apply on any of the
panels available from the Tools and Insert menus/toolbars.
•
Commands issued in the Command Editor dialog box.
•
Mesh import, delete, and transformation operations.
This chapter describes:
5.1. New Session Command
5.2. Start Recording and Stop Recording Commands
5.3. Play Session and Play Tutorial Commands
5.1. New Session Command
To record your actions in CFX-Pre in a session file:
1.
Select Session > New Session. This opens the Set Session File dialog box, where you can enter a file
name for your session file. Once you have saved the file, it becomes the current session file.
Note
This command is available only when a session file is not currently being recorded.
2.
Browse to the directory in which you want to create the session file, and then enter a name for the
file ending with a .pre (CFX-Pre) extension.
3.
Click Save to create the file.
4.
To start recording to the session file, select Session > Start Recording.
5.
To stop recording to the session file, select Session > Stop Recording.
Important
Session files must not contain > undo commands. These commands would produce errors
when playing back the session file.
If you create more than one session file during a CFX-Pre session, the most recently created file is the
current session file by default. You can set a different file to be the current session file by selecting an
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
51
Chapter 5: CFX-Pre Session Menu
existing file from the New Session > Set Session File window and then clicking Save. Because the file
exists, a warning dialog box appears:
•
If you select Overwrite, the existing session file is deleted and a new file is created in its place.
•
If you select Append, commands will be added to the end of the existing session file when recording
begins.
Note
By default, CFX-Pre does not continuously write commands to a session file while you are
working on your simulation. You can change a setting in Edit > Options so that a session
file is recorded by default. If a session file is being recorded by CFX-Pre, whether by default
or intentionally, a new session file cannot be recorded.
5.2. Start Recording and Stop Recording Commands
The Start Recording action activates recording of CCL commands issued to the current session file. A
session file must first be set before you can start recording (see New Session Command (p. 51)).
Stop Recording terminates writing of CCL commands to the current session file. You can start and stop
recording to a session file as many times as necessary.
5.3. Play Session and Play Tutorial Commands
A session file is a record of the actions performed during a CFX-Pre session, saved to a file when you
have defined a session file name and have clicked Session > Start Recording. By default, this file is
stored in your working directory.
A tutorial file is a record of the actions performed during a CFX-Pre tutorial; you can find tutorial files
provided by ANSYS in <CFXROOT>/examples.
This section describes:
•
Play Session Command (p. 52)
•
Play Tutorial Command (p. 53)
5.3.1. Play Session Command
After you have recorded a session file, you can select Session > Play Session, which opens the Play
Session File dialog box in which you can select the session file to play. The commands listed in the
selected session file are then executed.
52
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Play Session and Play Tutorial Commands
Important
If a session file is played while a current simulation is open, existing data will be lost in the
following situations:
•
If the session file starts a new simulation (that is, if it contains a >load command), then the
current simulation is closed without saving.
•
If the session file does not contain a >load command, the behavior is the same as importing
a CCL file using the Append option. For details, see Append or Replace (p. 35). Existing objects
with the same name as objects defined in the session file are replaced by those in the session
file.
To play a session file:
1.
From the menu bar, select Session > Play Session.
2.
Browse to the directory containing the session file and select the file you want to play.
3.
Click Open to play the session file.
Note
You can play session files in stand-alone CFX-Pre, but not in CFX-Pre in ANSYS Workbench.
5.3.2. Play Tutorial Command
Selecting Session > Play Tutorial opens the Play Session File dialog box where you can select a tutorial session file (.pre) to play from the examples directory of your CFX installation. The commands
listed in the selected tutorial session file are then executed.
Tutorial session files cannot be played while other simulations are open.
Note
You can play tutorial session files in stand-alone CFX-Pre, but not in CFX-Pre in ANSYS
Workbench.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
53
54
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 6: CFX-Pre Insert Menu
The Insert menu enables you to create new objects, such as domains or boundary conditions, or to
edit existing objects.
Tip
You are also able to create objects from shortcut menus in some contexts.
The settings specified in the various Insert menu panels correspond to all the data displayed in the
tree view. In many cases, the name of the new object can be specified. This name must be no more
than 80 characters in length.
Valid Syntax for Named Objects Any of the following characters are allowed in names of objects
in CFX-Pre: A-Z a-z 0-9 <space> (however, the first character must be A-Z or a-z). Multiple
spaces are treated as a single space character, and spaces at the end of a name are ignored.
In general, object names must be unique within the physics setup.
Analysis
Creates a new Flow Analysis in the Outline tree under Simulation. This enables you to define a steadystate analysis or a transient analysis.
Analysis Type
Specifies a steady-state or a transient analysis (in the analysis you select, when multiple analyses are
available). Steady-state analyses are used to model flows that do not change over time, while transient
analyses model flows that are time-dependent. For details, see Analysis Type (p. 101).
Domain
Creates new fluid and solid domains (in the analysis you select, when multiple analyses are available).
These are the bounding volumes within which your CFD analysis is performed. You can create many
domains in CFX-Pre and each can be stationary or rotate at its own rate, using different mesh element
types. For details, see Domains (p. 105).
Boundary
Sets the conditions on the external boundaries of a specified domain in a selected analysis. In CFX-Pre,
boundary conditions are applied to existing 2D mesh regions. For details, see Boundary Conditions (p. 149).
Subdomain
Creates subdomains, which are volumes within a specified domain in a selected analysis that are used
to create volumetric sources. For details, see Subdomains (p. 181).
Source Point
Creates sources of quantities at a point location within a specified domain in a selected analysis. For
details, see Source Points (p. 177).
Domain Interface
Connects fluid domains together (in the analysis you select, when multiple analyses are available). If a
frame change occurs across the interface, you have the choice of using a frozen rotor, stage, or transient
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
55
Chapter 6: CFX-Pre Insert Menu
rotor-stator model to account for the frame change. You can also take advantage of domain interfaces
to produce periodic connections between dissimilar meshes. For details, see Domain Interfaces (p. 137).
Global Initialization
Sets values or expressions for the global initial conditions (across all domains in the analysis you select,
when multiple analyses are available). Domain specific initialization is set through the domain forms. In
CFX-Pre, you can set linearly varying conditions from inlet to outlet using the initialization forms. For
details, see Initialization (p. 167).
Coordinate Frame
Creates and edits coordinate frames. A Cartesian coordinate frame exists by default, but other Cartesian
frames can be made. For details, see Coordinate Frames in the CFX-Solver Modeling Guide and Coordinate
Frames (p. 255).
Material / Reaction
Creates and modifies materials and reactions. For details, see Materials and Reactions (p. 259).
CFX-RIF
Inserts a flamelet library defined using CFX-RIF, a type of library generation software. For details, see
CFX-RIF in the CFX-Solver Modeling Guide.
Regions: Composite Region / Primitive Region
Composite regions can be created from basic primitive regions that are imported with a mesh. The Regions
details view supports union and alias operations. This enables you to manipulate existing 2D and 3D
regions without returning to the mesh generation software package. The creation of new regions is
limited by the topology of the existing primitive regions; therefore, you must still create appropriate
regions in the mesh-generation software package.
You can specify physics on either a primitive region, a composite region, or a mixture of both.
For details, see Regions (p. 95).
Additional Variable
Under Expressions, Functions and Variables, Additional Variable creates and modifies additional
solution variables. For details, see Additional Variables (p. 275).
Expression
Under Expressions, Functions and Variables, Expression creates and generates expressions using the
CFX Expression Language (CEL). For details, see Expressions (p. 281).
User Functions
Under Expressions, Functions and Variables, User Function creates 1D and cloud of points interpolation
functions. The interpolation functions are typically used to set boundary and initialization values in addition to profile data interpolation functions. For details, see User Functions (p. 287).
User Routines
Under Expressions, Functions and Variables, User Routine creates User CEL, Junction Box, and Particle
User Routines. For details, see User Routines (p. 293).
Solver: Solution Units
Sets the solution units used by the CFX-Solver (in the analysis you select, when multiple analyses are
available). These are the units that your results will appear in. For details, see Units and Dimensions (p. 193).
Solver: Solver Control
Controls the execution of the CFX-Solver (in the analysis you select, when multiple analyses are available).
This includes timestep and convergence details, as well as the choice of advection scheme. For details,
see Solver Control (p. 199).
56
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Solver: Output Control
Controls output from the CFX-Solver, including backup and transient results file creation (in the analysis
you select, when multiple analyses are available). For details, see Output Control (p. 213).
Solver: Mesh Adaption
Controls if and how the mesh will be automatically refined during the solution (in the analysis you select,
when multiple analyses are available). This technique can be used to refine the mesh to a particular flow
feature whose location is unknown prior to starting the analysis, such as a shock wave. For details, see
Mesh Adaption (p. 245).
Solver: Expert Parameter
Provides advanced control of the CFX-Solver (in the analysis you select, when multiple analyses are
available). For most analyses, you do not need to use expert parameters. For details, see Expert Control
Parameters (p. 253).
Solver: Execution Control
Enables you to define how the CFX-Solver is to be started for a simulation. See Execution Control (p. 299)
for details.
Configurations: Configuration / Termination Control
Simulation controls enable you to define the execution of analyses and related tasks such as remeshing
in the simulation. Specific controls include definitions of global execution and termination controls for
one or more configurations. See Configurations (p. 307) for additional information.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
57
58
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 7: CFX-Pre Tools Menu
The Tools menu provides access to the following:
7.1. Command Editor
7.2. Expand Profile Data
7.3. Initialize Profile Data
7.4. Macro Calculator
7.5. Solve
7.6. Applications
7.7. Quick Setup Mode
7.8.Turbo Mode
7.1. Command Editor
Displays and edits the CCL definition of objects, and as well issues commands directly to CFX-Pre. For
details, see Command Editor Dialog Box (p. 335).
7.2. Expand Profile Data
When setting up a boundary profile for a turbomachinery case (such as a transient blade row case involving an inlet disturbance), it is sometimes convenient to use a profile that wraps completely around
the machine axis.
Given an existing profile data file that describes, in Cartesian coordinates, a section that possesses rotational periodicity around a Rotation Axis, you can use the Expand Profile Data dialog box to obtain
a new profile file that contains a 360° profile. The input profile is replicated about the specified axis in
the positive rotational direction (according to the right-hand rule). The number of replications required
is given by the ratio of the specified Passages In 360 and Passages In Profile settings.
Note
Vector data is rotated in terms of both direction and position (while point data is rotated
only in terms of position).
Note
If a non-integer number of replications is needed to obtain a 360° profile, then the data for
the last replicated portion is truncated and a gap is left. The gap is positioned to be as far
away from the original profile as possible.
To expand profile data:
1.
Select Tools > Expand Profile Data.
The Expand Profile Data dialog box appears.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
59
Chapter 7: CFX-Pre Tools Menu
2.
Set Data File To Expand to the name of the current profile file.
You may use the file browser for this purpose, by clicking Browse
3.
.
Set Write To Profile to the name of the file that will hold the expanded profile.
You may use the file browser for this purpose, by clicking Browse
.
4.
Set Passages in Profile to the number of passages that the current profile models.
5.
Set Passages in 360 to the number of passages in a complete 360° revolution.
6.
Set Rotation Axis to the rotation axis around which the profile rotates.
7.
Click OK to begin the operation.
8.
When finished, click Close to close the dialog box.
7.3. Initialize Profile Data
Imports data from a file to use a profile boundary condition. For details, see Initializing Profile Data (p. 152).
7.4. Macro Calculator
The macro calculator in CFX-Pre is very similar to the one in CFD-Post. For details, see Macro Calculator
in the CFD-Post User's Guide. There are some minor differences between the two, however. For instance,
an additional widget type, Location, is available in the CFX-Pre macro calculator. This enables the
selection of mesh regions within the macro. An example of how to use this widget type is:
#
#
#
#
#
#
#
#
#
#
Macro GUI begin
macro name = StaticMixer
macro subroutine = test
macro report file = test_report.html
macro parameter = Domain Location
type = Location
value list = 3d composites, 3d primitives
A number of standard lists are available for this widget. The valid value list entries are as follows:
•
2d primitives / 3d primitives: all primitive 2D and 3D regions for the model
•
internal 2d primitives: all primitive 2D regions that are internal to the model
•
composites: all composite regions
•
2d composites / 3d composites: all 2D and 3D composite regions
•
assemblies: all assemblies
Also, predefined macros are not supplied for CFX-Pre the way they are in CFD-Post. For details, see
Predefined Macros in the CFD-Post User's Guide.
7.5. Solve
Available in stand-alone mode for the current definition of the case, you can use the Solve option to:
•
from Start Solver;
–
60
select Define Run to write the CFX-Solver input file and start the CFX-Solver Manager,
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Turbo Mode
–
select Run Solver to write the CFX-Solver input file and start the CFX-Solver,
–
select Run Solver and Monitor to write the CFX-Solver input file and start both the CFX-Solver
and the CFX-Solver Manager
.
•
from View in CFD-Post, write the CFX-Solver input file and start CFD-Post
•
from Write Solver Input File, write the CFX-Solver input file.
7.5.1. Write Solver Input File Command
A CFX-Solver input file contains information (such as physics, mesh) required to execute a case in CFXSolver to solve physics.
1.
.
Select Tools > Solve > Write Solver Input File from the menu bar or click Write Input Solver File
The Write Solver Input File dialog box appears.
2.
Select a location to which to save the file.
3.
Under File name, type the name of the file.
4.
Click Save.
If the file name assigned is the same as an existing file name in the same location, select Overwrite
to overwrite the original file, Re-select to specify a new file name, or Cancel to cancel the writing
of the .def file.
7.6. Applications
Available in stand-alone mode, these commands immediately load CFX-Solver Manager or CFD-Post.
7.7. Quick Setup Mode
Quick Setup Mode is used to quickly specify cases that involve simple physics. For details, see Quick
Setup Mode (p. 319).
7.8. Turbo Mode
Set up certain turbomachinery cases quickly and easily using Turbo mode. For details, see Turbomachinery
Mode (p. 323).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
61
62
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 8: CFX-Pre Extensions Menu
The Extensions menu provides access to any customized extensions available to CFX-Pre.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
63
64
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 9: Importing and Transforming Meshes
CFX-Pre can import meshes from a wide range of sources. Once imported, you can position and scale
each mesh as required (as described in Transform Mesh Command (p. 82)).
You can import more than one mesh per CFX-Pre simulation. After you have imported all your meshes
and created all your domains, the domains should be joined together, either by gluing them together,
or by using domain interfaces. For details, see Gluing Meshes Together (p. 88) and Domain Interfaces (p. 137).
This chapter describes:
9.1. Importing Meshes
9.2. Mesh Tree View
9.3. Deleting Meshes and Mesh Components from the Tree View
9.4.Transform Mesh Command
9.5. Gluing Meshes Together
9.6. Mesh Editor
9.7. Render Options
9.8. Mesh Topology in CFX-Pre
9.9. Advanced Topic: cfx5gtmconv Application
Additional information on assemblies, primitive regions, composite regions, and the regions that are
created when importing meshes is available in Mesh Topology in CFX-Pre (p. 91).
9.1. Importing Meshes
Meshes are imported via the Import Mesh dialog box, which is accessible in several ways:
•
By selecting File > Import > Mesh
•
By right-clicking the Mesh branch in the tree view and selecting Import Mesh from the shortcut menu
•
By selecting Browse
when setting the file name for a mesh (for example, in Turbomachinery mode).
You can multi-select mesh files by holding the Ctrl key while you click the file names.
Import options may appear on the Import Mesh dialog box, depending on the type of mesh being
imported. Some common import options are described next. Other options that are specific to particular
mesh formats are discussed in Supported Mesh File Types (p. 67).
9.1.1. Importing Multiple Meshes
It is possible in CFX-Pre to import multiple mesh file to construct an appropriate model for your simulation. Each mesh imported is represented in the Mesh part of the Outline tree by a unique identifier
based on the name of the mesh file imported.
In general, a mesh file is represented by the file name of the file imported without any preceding path
(for example, if you imported C:\Directory\File.cmdb, this will be represented in the tree as
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
65
Chapter 9: Importing and Transforming Meshes
File.cmdb). If after transforming the file name in this way the transformed name is already present
in the tree, either because this is an earlier import of the same file or another file with the same name
has been imported from a different directory, the new file will be labelled with a suffix, such as
File.cmdb(1) for example.
If multiple mesh files are transformed in such a way that the result of the transformation glues the two
files together or the files are explicitly glued together, the original mesh file entries will no longer appear
under the Mesh entry as file names, but the resulting Principal 3D regions will appear under a Merged
Meshes item under Mesh.
9.1.2. Common Import Options
9.1.2.1. Mesh Units
This option is displayed depending on the file type selected. The units selected on the Import Mesh
dialog box are the units used to import the mesh and are the default units for transforming mesh assemblies using the Mesh Transformation Editor dialog box. These units are local to the mesh import
and transformation options and do not affect either the solution units or the units set under Edit >
Options. For details, see:
•
Setting the Solution Units (p. 197)
•
Units (p. 48).
CFX-Pre will attempt to determine the units used in a mesh file and convert them to the specified units
during import. For example, a mesh of 1000 units long, with units in the mesh file of mm, will appear
in CFX-Pre as 1 m long, if units of m are set on the Import Mesh dialog box. If CFX-Pre cannot determine
the units used in the mesh file, then in this example the mesh would appear as 1000 m long.
9.1.2.2. Assembly Prefix
This is the name used to prefix the assemblies that are created when the mesh is imported. A number
suffix is added to the second, and any subsequent meshes, using the same assembly prefix, so that
each assembly is named uniquely.
9.1.2.3. Primitive Strategy
This setting enables you to control the names of split regions.
The following options are available:
Standard - Select this option so that the name of each split region starts with “Primitive 2D” or
“Primitive 3D”. For example, this option splits “My Region Name” into “Primitive 2D A” and “Primitive
2D B”.
Derived - Select this option so that the name of each split region is derived from the name of the
region that is being split. For example, this option splits “My Region Name” into “My Region Name A”
and “My Region Name B”.
9.1.2.4. Ignore Invalid Degenerate Elements
If your mesh import fails because of invalid degenerate elements, then you can enable this toggle.
However, your mesh may not be valid for use in the CFX-Solver. You may have to fix or remove the
degenerate elements in the software used to generate the mesh.
66
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
9.1.2.5. Duplicate Node Checking
Duplicate Node Checking is off by default and, in general, need not be selected.
Nodes within the specified relative tolerance are equivalenced into a single node (duplicate node removal). The default tolerance of 1e-04 is sensible and you should not change it. The relative tolerance
is based on the local mesh length scale, so by default nodes within 0.001% of the average mesh edge
length of all edges connected to a node will be equivalenced.
9.1.3. Supported Mesh File Types
Mesh file types supported by CFX-Pre are:
9.1.3.1. ANSYS Meshing Files
9.1.3.2. CFX-Mesh Files
9.1.3.3. CFX-Solver Input files
9.1.3.4. ICEM CFD Files
9.1.3.5. ANSYS Files
9.1.3.6. FLUENT Files
9.1.3.7. CGNS Files
9.1.3.8. CFX-TASCflow Files
9.1.3.9. CFX-4 Grid Files
9.1.3.10. CFX-BladeGenPlus Files
9.1.3.11. PATRAN Neutral Files
9.1.3.12. IDEAS Universal Files
9.1.3.13. GridPro/az3000 Grid Files
9.1.3.14. NASTRAN Files
9.1.3.15. Pointwise Gridgen Files
9.1.3.16. User Import
Note
Users of the DesignModeler, Meshing application, and ANSYS CFX products should refer to
Meshing: Named Selections and Regions for CFX in the Meshing User's Guide for important
information about region definitions.
9.1.3.1. ANSYS Meshing Files
ANSYS Meshing files of the form .cmdb and .dsdb can be imported.
Note
•
You must have ANSYS Workbench installed in order to import ANSYS Meshing files (.cmdb
and .dsdb) into CFX-Pre or CFD-Post.
•
CFX-Pre does not support importing meshes from .cmdb files generated by the Meshing
application prior to Release 11.0.
You can specify an assembly prefix. For details, see Common Import Options (p. 66).
There are import settings that are specific to ANSYS Meshing files.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
67
Chapter 9: Importing and Transforming Meshes
The Model(s) To Read setting defaults to All, which specifies that all models are to be imported from
the ANSYS Meshing file. However, if you load a cmdb/dsdb file that has multiple models in it, you can
specify which models to load.
Note
You must click
next to the Model(s) To Read setting before the other models will appear.
9.1.3.1.1. Named Selections
Named selections are aliases for collections of regions. When importing a mesh, you can preserve these
named selections based on where they were created:
•
CFX Mesh Names for regions defined in CFX-Mesh.
•
Simulation Names for named selections generated in the Mechanical application and ANSYS
Workbench Meshing.
•
Symmetry Names for named selections of 2D symmetry and periodic regions generated in the
Mechanical application and ANSYS Workbench Meshing.
•
Part Manager Names for named selections generated in DesignModeler or other CAD systems
that are not written to the .cmdb file by the meshing application.
•
Fall Back to Part Manager Names for using named selections generated directly by DesignModeler
or other CAD systems as a fall back if no CFX-Mesh, Simulation or Symmetry named selections are
found.
9.1.3.1.2. Contact Detection Settings
The Contact check box, when selected, makes contact detection settings available.
When importing ANSYS Mesh files (.cmdb / .dsdb files), it is possible to select Detection Method >
Read to read contact information from the file or to select Detection Method > Detect to use the
contact detection methods to determine whether regions within the mesh are “in contact” with each
other. CFX-Pre uses the Mechanical application contact detection methods to determine which mesh
volumes should be placed within each mesh assembly and which 2D regions are connected.
The Detection Between setting can be set to Bodies or All Contact. When using the Bodies option,
2D regions will be matched between different bodies. This is the default option and should result in
bodies that are “close” to one another being placed in the same mesh assembly. If automatic domain
interface generation is selected, interfaces will be generated between such regions. When using the All
Contact option, CFX-Pre will still recognize contact between discrete bodies, but in addition, it will look
for contact between 2D regions within the same “body”, or “volume”. This can result in unexpected
behavior, such as adjacent surfaces being considered “in contact” and hence this is not the default option,
but in some cases, where there are non-matched 2D mesh regions within a mesh volume, it can help
generate “internal” interfaces.
The tolerance that is used in detecting contact can be altered and it is possible to define it relative to
the local geometry size, or as an absolute spatial value.
If CFX-Pre is set to read contact information from the file, then it will import only connections that
connect two single regions. Connections connecting multiple regions to a single region, or multiple
regions to multiple regions, will be ignored. Also, contact detection works only within a single file; CFXPre will not read or detect contact between meshes that are imported from different files.
68
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
If the Meshing application is set to generate connections automatically, you can set the Global Contact
Setting option to Group By > None to generate only single region to single region connections. For
more details, see Generation of Contact Elements in the Meshing User's Guide.
9.1.3.2. CFX-Mesh Files
The CFX-Mesh (.gtm, .cfx) files are native for CFX-Pre; therefore, all information in such a file is read
in by the import process. There are no options needed to control the reading of these files.
Note
Only .cfx files that are version 11.0 or newer are supported.
9.1.3.3. CFX-Solver Input files
CFX-Solver files include CFX-Solver input (.def), results (.res), transient results (.trn), and backup
(.bak) results files. There are no options specific to importing CFX Def/Res, files but the general advanced
options are described in Common Import Options (p. 66).
For additional information on the regions created in CFX-Pre when CFX-Solver files are imported, see
Mesh Topology in CFX-Pre (p. 91).
9.1.3.4. ICEM CFD Files
ICEM CFD files are of the form .cfx, .cfx5, .msh. There are no import options specific to ICEM CFD
files; however the Common Import Options (p. 66) apply.
9.1.3.5. ANSYS Files
ANSYS files are of the form .cdb or .inp. There are no import options specific to ANSYS files; however
the Common Import Options (p. 66) apply.
Only .cdb files can be imported into CFX-Pre. If you have an ANSYS .db file, you can convert it to a
.cdb file in ANSYS by:
1.
Opening the ANSYS database in ANSYS.
2.
Issuing the ALLSEL command to select everything.
3.
Issuing the CDWRITE, DB command to write the .cdb file.
To get a list of all element types (ET)/keyops(KEYOP) that are supported by mesh import, you can
run the following from the operating system command line:
<CFXROOT>/bin/<OS>/ImportANSYS.exe -S
Note
Before executing the CDWRITE command, verify that the data base has a separate named
component of 2D MESH200 elements for each surface that will require a boundary condition.
Delete any MESH200 elements that are not members of named components. To define specific 3D regions, create a 3D named component of 3D elements. The component names will
appear in CFX-Pre as defined regions.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
69
Chapter 9: Importing and Transforming Meshes
9.1.3.6. FLUENT Files
FLUENT files of the form .cas and .msh can be imported.
Note
When importing meshes from FLUENT files in CFX-Pre, Release 12.0 (or later), the topology
and naming of regions may not be the same as those generated by importing these
meshes into previous releases. As a result, session files generated in CFX-Pre Release,
11.0 (or earlier) that import meshes from FLUENT files may generate errors when loaded
into CFX-Pre, Release 12.0 (or later).
9.1.3.6.1. Override Default 2D Mesh Settings
9.1.3.6.1.1. Interpret 2D Mesh as
9.1.3.6.1.1.1. Axisymmetric
This option enables you to create a 3D geometry by extruding a 2D geometry through a specified rotation
angle in the third dimension.
Number of Planes:
This value enables you to create additional planes, arranged in the extruded direction, to create a 3D
problem. This will increase the number of elements in the extruded direction, but does not change the
enclosed angle of the mesh.
Angle (deg):
This is the angle through which the original 2D mesh is extruded.
Remove Duplicate Nodes at Axis:
This check box enables you to choose to have the duplicate node removed from the axis of an axisymmetric case upon import.
9.1.3.6.1.1.2. Planar
This option enables you to create a 3D geometry by linearly extruding a 2D geometry in the third dimension.
Extrude Distance:
This is the distance through which the geometry is extruded in the third direction.
For further advice on how to model 2D problems in CFX, refer to Modeling 2D Problems in the CFXSolver Modeling Guide.
9.1.3.7. CGNS Files
CGNS files are of the form: .cgns. Applicable import options are:
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67)
70
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
9.1.3.7.1. Importing CGNS files into CFX
9.1.3.7.1.1. Method
Mesh data contained within CGNS files can be read into a CFX-Pre after a new case has been created
or an existing case has been opened. To read the CGNS file, select the file to import and, if necessary,
alter the options used to import the mesh under the Advanced Options section.
Further information on importing files is contained within the standard documentation.
9.1.3.7.1.2. Base (Base_t)
The top-level object in a CGNS file is a container called a base, a CGNS file that can contain multiple
bases. What a base contains is user defined so that CFX-Pre allows all bases to be read by one import,
or single bases to be read by separate imports.
9.1.3.7.1.3. Zone (Zone_t)
Each base contains one or more zones. For each base read, the import process reads all zones, provided
they are 3D dimensional (structured or unstructured zones are supported).
•
Grids can be read in single or double precision.
•
Zones may be specified in Cartesian or Cylindrical coordinates. Other coordinate systems are not currently
supported.
9.1.3.7.1.4. Elements (ElementSection_t)
Element sections can be imported as regions of interest or ignored. How this is done is controlled by
the user interface - you must understand which behavior you want to see. It may be useful to import
the element sections, for example, if the file has been written with all faces (2D elements) in a boundary
patch as a separate element section, which could be useful for setting up the problem in CFX-Pre.
Similar scenarios can be imagined in 3D element sections or even mixed element sections.
9.1.3.7.1.5. Element Types Supported
Supported 3D elements (TETRA_4, PYRA_5, PENTA_6 and HEXA_8). Other 3D elements can be read but
are reduced to the lower order elements (that is, TETRA_10 is translated to TETRA_4 and then this is
imported).
Supported 2D elements (TRI_3 and QUAD_4). Other 2D elements can be read but are reduced to the
lower order elements (that is, TRI_6 is translated to TRI_3 and then is imported).
The vertices of 2D elements should ideally be based on the node indices as are used for to define the
3D elements.
It is preferable to define 2D elements with parent information so that mapping from 2D elements to
3D elements does not have to be determined by the process, therefore, reducing import times.
9.1.3.7.1.6. Boundary Conditions (BC_t)
Boundary conditions are processed but physical setup information (for example, equations) is ignored.
The facility for importing the CGNS files into CFX (CFX-Pre) is a mesh (grid) importer, not a physics importer.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
71
Chapter 9: Importing and Transforming Meshes
No physics information is imported. Boundary condition locations are read because the collections (regions) of mesh elements the condition is defined upon are required for ease of use and correct physics
setup in CFX.
It is quicker to read boundary conditions when they are defined as a range of elements (ElementRange)
or a list of elements (ElementList), rather than a range of nodes (PointRange) or a list of nodes
(PointList). The latter may also be read, but the nodes referenced must also be used by higher-dimension elements (for example, 3D elements) for correct interpretation.
9.1.3.7.1.7. Families (Family_t, FamilyBC_t, FamilyName_t)
Families are read and, in general, imported as composite regions (groupings) of underlying primitive
regions.
9.1.3.7.1.8. Grid Connectivity (GridConnectivity_t and GridConnectivity1to1_t)
Grid connectivity can be read but with certain restrictions.
•
If the interface is read from a GridConnectivity1to1_t node or is a read from a GridConnectivity_t node and is of type Abutting1to1, importing of the node mapping is attempted.
•
If the node mapping cannot be established or the user requests that the two sides of the interface are
imported as separate regions.
Other interface types are always imported as two separate regions.
9.1.3.7.1.9. CGNS Data Ignored
The CGNS Mid Level Library Documentation Page (http://www.grc.nasa.gov/WWW/cgns/CGNS_docs_current/midlevel/index.html) details the interface used for reading CGNS files within CFX-Pre. The following
high level headings used within the document are ignored.
•
Simulation Type
•
Descriptors
•
Physical Data
•
Location and Position1
•
Auxiliary Data
•
Solution Data
•
Equation specification
•
Time Dependent Data
9.1.3.7.2. Prefix regions with zone name
This check box determines whether or not each imported region is prefixed with the name of the zone
within which it is defined.
1
Rind Data is processed but not imported.
72
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
9.1.3.7.3. Create Regions From: Element Sections
Each element section that specifies the topology of elements within the CGNS file may or may not imply
a grouping of these elements that is important. If the grouping of elements within each element section
is important, this option should be selected so the grouping is preserved within CFX-Pre.
Element sections can be 2D or 3D or a mixture of both, and as such can form 3D regions or 2D regions
in CFX-Pre.
The way they are grouped depends on vendor interpretation of the CGNS standard.
9.1.3.7.4. Create Regions From: Boundary Conditions
This check box determines whether or not to import boundary conditions as regions.
9.1.3.7.5. Create Regions From: Families
This check box determines whether or not to import families of elements, or faces as regions.
9.1.3.7.6. Create Regions From: Connectivity Mappings
This check box determines whether or not to import zone interfaces (that is, 1-to-1 and GGI connections)
as regions.
9.1.3.7.7. Example of Create Regions From
Consider a CGNS file with one zone, Zone 1, comprising of four elements sections (ES1 and ES2 defining the 3D elements, and ES3 and ES4 defining the 2D elements). It also contains 2D boundary
conditions BC1 and BC2.
These element sections, ES1 and ES2, could be, for example, comprised of hexahedral elements in
ES1 and tetrahedral elements in ES2. In this case, the groupings of elements into the first two element
sections appears to be due to their topological identity. However, this may or may not be the case and
you must decided as to whether importing these groupings is important.
In this case, it may be that ES1 and ES2 should be combined by clearing the Create Regions From:
Element Sections option. Another possibility is that ES1 may be a subregion of mesh that should be
kept separate (that is, it will be set up as a subdomain). If that were the case, Element Sections should
be selected.
If BC1 is defined on all the faces in ES3 and BC2 is defined on all the faces in ES4, then it will probably
not be necessary to select Boundary Conditions if Element Sections is selected, as this would introduce
complexity in the region definitions (that is, composites would be defined). However if the groupings
of ES3 and ES4 are different from the groupings in the boundary conditions then Create Regions
From: Boundary Conditions should be selected.
9.1.3.7.8. Read Only One CGNS Base
When this toggle is selected, a mesh is read from a single base specified by the CGNS base to read
number. If your CGNS file contains only a single base, you should leave the number set to 1. If it contains
more than one base, you should specify the base number from which to read. If the base number specified does not exist, an error will be raised. If it does not contain a valid mesh then a mesh will not be
imported.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
73
Chapter 9: Importing and Transforming Meshes
Note
You must click
before you can specify which base to read.
If you disable the Read Only One CGNS Base toggle, then CFX-Pre will look for meshes in all bases
and import them. If multiple assemblies are imported and they overlap, then the mesh will be invalid
within CFX-Pre unless assemblies are transformed in some way.
For details, see SplitCGNS.exe in the CFX Reference Guide. This is a program that splits a CGNS file into
multiple problem files.
9.1.3.8. CFX-TASCflow Files
CFX-TASCflow mesh files are of the form .grd or are simply named grd. You may receive warning
messages when importing a CFX-TASCflow mesh file: these will usually tell you which regions have not
been imported. The sections below indicate the situations when a warning message may occur.
•
If Convert 3D Region Labels to Regions is selected, then the 3D Region labels in the .grd file are imported as individual 3D Regions. The default setting omits all 3D Region labels.
•
If Ignore One-to-One Connections is selected, then one-to-one contiguous grid connections are deleted
on import. You would then have to recreate the connections in CFX-Pre. There are very few cases when
you would want to enable this toggle.
•
Select the file type for the imported mesh from the GRD File Format Type drop-down. You can select
from Formatted, Unformatted or Unknown. If you select Unknown, CFX attempts to determine
the file format before importing the mesh.
•
If Retain Block Off is selected, then “user defined” elements that are blocked off in the mesh file are
not imported into CFX-Pre. If not selected, then “user defined” objects are ignored and the elements
are included in the imported mesh (rarely desired).
Additional information is available in:
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67).
9.1.3.8.1. Convert 3D Region Labels to Regions
This toggle controls 3D region import from the .grd file only. When selected, 3D regions in the .grd
file will be imported into separate 3D primitives in CFX-Pre. If you do not select this option, all mesh
elements will be imported into a single 3D primitive that is uniquely named by the import process. 3D
regions defined in the .gci and .bcf files are always imported.
9.1.3.8.2. Grid Connections Processed (in the .grd file)
When importing CFX-TASCflow meshes, the only grid connections that are imported automatically are
“many-to-one” contiguous topology connections that are specified as one-to-one node pairings.
“Many-to-one” contiguous topology connections that involve any number of many-to-one node
groupings are ignored and a warning message is issued; however, the two sides of the connection are
preserved as a pair of 2D regions on which a GGI Connection can be defined. You should recreate the
connection in CFX-Pre using a Fluid-Fluid Domain Interface. For details, see Creating and Editing a Domain
Interface (p. 137). In some cases, if you have not created regions in CFX-TASCflow on each side of an
74
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
interface, you will not be able to recreate it in CFX-Pre because there will be no region available for
selection. If this occurs, you should explicitly create regions in CFX-TASCflow before importing the mesh
into CFX-Pre.
Important
Some ANSYS TurboGrid grids contain many-to-one node groupings. These will not be imported
into CFX-Pre. You need to know if your grid contains these connections and then recreate
them in CFX-Pre using Fluid-Fluid Domain Interfaces.
“Many-to-one” periodic topology connections are always removed with a warning message issued. You
should recreate the connections using a periodic domain interface. For details, see Creating and Editing
a Domain Interface (p. 137).
The regions associated with periodic boundary conditions are imported, but you will need to assign
the regions to a periodic domain interface.
9.1.3.8.3. Grid Embedding
Embedded grids, along with the parent grid, are automatically imported into separate assemblies in
CFX-Pre. The many-to-one topology connections on the interface between the embedded grid and the
parent grid will be removed and a warning issued. You will need to create fluid-fluid domain interfaces
between the embedded grid and the parent grid. For details, see Creating and Editing a Domain Interface (p. 137).
9.1.3.8.4. Retain Block-off
The Retain BlockOff toggle is selected by default. There is no harm in leaving this on, but it is not required unless user defined block-off is defined in the .bcf the file, and you want it to remain blockedoff (ignored).
Porous and CHT objects in the .bcf file are ignored, and must be manually created in CFX-Pre after
importing the grid. You should make sure that a 3D volume region was defined in the grd file for the
porous or CHT object location prior to import.
By default, CFX-Pre will look in the same directory as the .grd file to locate the .bcf file. If the .bcf
file is located elsewhere, you can browse and select the file.
9.1.3.8.5. Regions in the .grd file
You should delete any regions from the .grd file that are not needed.
If necessary, you can force all “user defined” regions to be included in a .grd file by executing the
following command at the TASCtool command prompt:
TASCtool{}: write grd all_regions_to_grd=on
This is usually not needed because you can import regions from the .gci file directly (see below).
Note that when faces are referenced by more than one named region, the import process will resolve
this conflict such that faces are not referenced by more than one region.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
75
Chapter 9: Importing and Transforming Meshes
9.1.3.8.6. Boundary Conditions in .bcf File
The regions associated with the boundary conditions defined in the .bcf file are imported into CFXPre. The boundary condition physics definitions are ignored and must be defined in CFX-Pre.
The CFX-TASCflow symmetry/slip boundary condition should be recreated as either:
•
A symmetry boundary condition for flat surfaces.
•
A wall boundary condition using the Free Slip option for curved surfaces.
9.1.3.8.7. Regions in the .gci File
Regions in the .gci file defined in (i, j, k) coordinates (such as boundary conditions) are imported if
the Use GCI file toggle is enabled on the Advanced Options tab. By default, CFX-Pre looks in the same
directory as the .grd file for the location of the .gci file. You should select the location of the .gci
file by clicking on the browse icon if it is located elsewhere.
Regions defined in physical space (x, y, z coordinates) are always ignored.
An alternative method for reading the .gci file is to force all regions to be included in the .grd file.
For details, see Regions in the .grd file (p. 75).
9.1.3.8.8. Importing CFX-TASCflow TurboPre MFR Grids
You can create multiple domains from a single .grd file if it contains multiple 3D regions or GGI connections. For an MFR grid, a separate assembly will be created for each noncontinuous grid region. This
enables a multiple frame of reference (MFR) case to be easily recreated in CFX-Pre from a single mesh
import.
Grids from CFX-TASCflow TurboPre usually contain many named regions that may not be required to
set up the problem in CFX-Pre. You might want to remove some of these regions before importing the
grid to speed up the import of the mesh and simplify the imported mesh.
In CFX-TASCflow TurboPre, you can create multiple copies of blade passages. The ‘open ends’ of the
machine section will use a periodic connection. These must be recreated in CFX-Pre using a periodic
domain interface. For details, see Creating and Editing a Domain Interface (p. 137). The internal connection
between blade passages can be connected in CFX-TASCflow TurboPre using an automatic periodic
boundary condition. If such a connection is used you will have to manually reconnect each passage in
CFX-Pre. You might therefore want to define a many-to-one topology connection for one-to-one grid
connections so that passages are connected by CFX-TASCflow TurboPre as topology connections (which
import immediately). For details, see Grid Connections Processed (in the .grd file) (p. 74).
9.1.3.8.9. Parameter File
CFX-TASCflow does not have units checking, whereas CFX-Pre does. Grid numbers will be imported
using the units specified on the Import Mesh dialog box. You should convert all units in the properties
and parameter files within TASCflow into SI units (kg, meter, second) prior to import.
9.1.3.9. CFX-4 Grid Files
CFX grid files are of the form .geo.
•
76
Select Split Symmetry Planes to split symmetry planes that exist in more than one region. For details,
see Split Symmetry Planes (p. 77).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
•
Select Import from Cylindrical Coordinates to transform a problem defined in cylindrical coordinates
into Cartesian coordinates for use in CFX-Pre. It should be selected for all CFX-4 problems that use cylindrical coordinates. For details, see Import from Cylindrical Coordinates (p. 77).
•
Select Block Interfaces to create 2D regions in CFX-Pre on block interfaces. For details, see Create 2D
Regions on (p. 77).
•
Import 2D axisymmetric mesh. For details, see Import 2D Axisymmetric Mesh (p. 78).
Other available options are:
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67)
9.1.3.9.1. Split Symmetry Planes
The Split Symmetry Planes option is on by default. Symmetry planes that are defined by more than
one CFX-4 region will be split so that each definition is imported. For example, a symmetry plane that
is defined on two sides of a 3D region will be split into regions named <regionname>1 and <regionname>2, and so on, where <regionname> is the original name of the symmetry plane in the CFX-4
file.
9.1.3.9.2. Import from Cylindrical Coordinates
CFX-Pre can import problems defined in Cylindrical Coordinate (x, r, ) form from CFX-4. The problem
is converted to Cartesian Coordinates (x, y, z) by the import process. The resulting CFX-Solver input file
will not be written in cylindrical coordinates. You must select the Import from Cylindrical Coordinates
option to successfully import a CFX-4 cylindrical coordinate problem.
Note
This is not the same as an axisymmetric problem. For details, see Import 2D Axisymmetric
Mesh (p. 78).
9.1.3.9.3. Create 2D Regions on
Block Interfaces
When this option is selected, named regions will be created on the interfaces between mesh blocks.
This can produce many regions in CFX-Pre, so it is usually better to define all the regions you require as
patches in CFX-4.
9.1.3.9.4. Create 3D Regions on
Fluid Regions (USER3D, POROUS)
In CFX-4, most 3D regions are classified as USER3D patches. Porous regions are treated in the same way
as USER3D regions when importing them into CFX-Pre. When the Fluid Regions (USER3D, POROUS)
toggle is not selected, these regions are not imported. When the toggle is selected, they are imported
as separate 3D regions. This toggle should be selected if you need the USER3D regions to create domains
and subdomains. You should disable it to simplify the regions created in CFX-Pre. If, in CFX-4, you have
created a USER3D region for the purpose of creating thin surfaces, you do not need to import the USER3D
region in CFX-Pre because thin surfaces can be defined without the need for a separate subdomain.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
77
Chapter 9: Importing and Transforming Meshes
9.1.3.9.5. Blocked Off Regions (SOLIDs)
•
If Fluid Regions (USER3D, POROUS) is not selected, and Blocked Off Regions (SOLIDs) is not selected,
then SOLID regions are blocked-off (that is, this part of the mesh is not imported).
•
If Fluid Regions (USER3D, POROUS) is not selected, and Blocked Off Regions (SOLIDs) is selected,
then SOLID regions are imported into the default 3D region created by the import process.
•
If Fluid Regions (USER3D, POROUS) is selected, and Import SOLID regions is toggled OFF, then
SOLID regions become blocked-off (that is, this part of the mesh is not imported).
•
If Fluid Regions (USER3D, POROUS) is selected, and Import SOLID regions is toggled ON, then SOLID
regions are imported as separate 3D regions (which can be useful for CHT simulations).
9.1.3.9.6. Conducting Solid Regions (SOLCONs)
•
These are regions defined as conducting solid regions in CFX-4. There is no way to completely ignore
SOLCON regions, they are always imported as either a separate region or as part of the parent region.
If you want to ignore these regions (that is, so that there is no flow), then they should be removed from
the CFX-4 mesh file using CFX-4 or with manual editing. Alternatively they can be imported but simply
not used to define a subdomain in CFX-Pre. The import behavior is described below:
–
If Fluid Regions (USER3D, POROUS) is not selected, and Conducting Solid Regions (SOLCONs)
is not selected, then SOLCON regions are imported as part of the “Assembly 3D” region.
–
If Fluid Regions (USER3D, POROUS) is not selected, and Conducting Solid Regions (SOLCONs)
is selected, then SOLCON regions are imported as separate 3D regions.
–
If Fluid Regions (USER3D, POROUS) is selected, and Conducting Solid Regions (SOLCONs) is not
selected, then SOLCON regions are imported as part of the regions in which they appear.
–
If Fluid Regions (USER3D, POROUS) is selected, and Conducting Solid Regions (SOLCONs) is selected, then SOLCON regions are imported as separate 3D regions and will be cut out of the parent
regions.
9.1.3.9.7. Import 2D Axisymmetric Mesh
You can enable this toggle if you want to import a mesh created as a 2D mesh on an axisymmetric
section in CFX-4. This is different to a mesh defined using cylindrical coordinates; however, it can also
use an (x, r, ) coordinate system. The CFX-4 mesh must be only 1 element thick in the k direction to
use this option.
The Number of Planes value enables you to create additional planes in the direction within the original 2D mesh to create a 3D problem. This will increase the number of elements in the k direction, but
does not change the extent of the mesh.
The Angle value should be the angle of the mesh section in degrees. Because the mesh is only one
element thick, then is the same for all nodes.
9.1.3.9.8. Importing MFR Grids
If you have a CFX-4 MFR case, it can easily be imported into CFX-Pre and recreated.
•
Each noncontinuous mesh section will be imported into a separate assembly.
•
Each USER3D region will be imported into a separate 3D primitive.
•
Both assemblies and 3D primitives can be used to create separate domains.
78
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing Meshes
9.1.3.10. CFX-BladeGenPlus Files
CFX-BladeGenPlus files are of the form .bg+. There are no options specific to importing CFX-BladeGenPlus
files. For details, see Common Import Options (p. 66).
9.1.3.11. PATRAN Neutral Files
PATRAN Neutral files are of the form .out.
•
Select Import Distributed Loads as 2D Regions to convert predefined distributed loads as 2D primitives
within CFX-Pre.
For details, see Common Import Options (p. 66).
9.1.3.12. IDEAS Universal Files
IDEAS Universal files are of the form .unv.
•
Select the entities, under IDEAS Universal Specific Options, to import from Permanent Groups.
For details, see Common Import Options (p. 66).
IDEAS mesh files contain groups of nodes, faces and/or elements. The groups can be normal groups or
permanent groups. The normal groups are imported into CFX-Pre as up to three separate regions, depending on the information available in the mesh file. These regions will be named:
•
<groupName>_Nodes
•
<groupName>_Faces
•
<groupName>_Elements
Only permanent groups of the selected types are imported into CFX-Pre. If overlapping regions are
imported, CFX-Pre will split them into distinct regions; therefore, you may not want to import all permanent group types.
9.1.3.13. GridPro/az3000 Grid Files
GridPro/az3000 ‘grid’ files are of the form .grid.
•
Select Include Periodic Regions to convert predefined periodic boundaries into 2D primitives on import.
•
Select Ignore Connectivity to import grid blocks as unconnected 3D primitives. Ignoring connectivity
does not equivalence nodes at grid block interfaces.
•
Select Import Grid Blocks as Subdomains so that for each predefined grid block, a separate 3D primitive is created.
•
Selecting Ignore Properties causes data in the properties file to be ignored. This includes boundary
conditions, 2D and 3D regions, and other data.
Additional information is available in:
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
79
Chapter 9: Importing and Transforming Meshes
9.1.3.14. NASTRAN Files
NASTRAN files can be imported.
•
When Include Subdomains is cleared, all mesh elements are merged into a single 3D primitive.
•
“Distributed loads” are pressure boundaries that, if imported, are used to generate 2D primitives in CFXPre. Select Import Loads as 2D Regions to import distributed loads.
Additional information is available in:
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67).
9.1.3.15. Pointwise Gridgen Files
Pointwise Gridgen files can be imported. There are no options available specific to the Pointwise Gridgen
format. For details, see Common Import Options (p. 66).
9.1.3.16. User Import
If you should require facilities for importing a mesh other than those available through the standard
Mesh Import forms, you can create your own customized mesh import program and make it available
through the Import Mesh forms. For details, see Volume Mesh Import API in the CFX Reference Guide.
If you have created your own mesh import program, it must be run from within CFX-Pre; one way of
doing this is by using the Import Mesh dialog box.
To run a custom import program using the Import Mesh dialog box:
1.
Open the Import Mesh dialog box.
For details, see Importing Meshes (p. 65).
2.
Set Files of Type to User Import(*).
3.
Select the file containing the mesh to import.
4.
Click Browse
ation.
5.
Under Exec Arguments, enter the command-line arguments that should be passed to the import
program.
6.
Set advanced options as required.
to browse to the location of the user executable file or enter its name under Exec Loc-
For details, see:
7.
•
Ignore Invalid Degenerate Elements (p. 66)
•
Duplicate Node Checking (p. 67)
Click Open.
CFX-Pre calls the custom import program with a command line that has the following form:
<user import executable> <executable arguments> <mesh file>
It is important therefore that the executable handles any arguments that are specified.
80
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Deleting Meshes and Mesh Components from the Tree View
If you usually use a particular import program, you can set it as the default import program by any one
of the following methods:
•
Specify the full path name of the import program, and other settings, in the Options dialog box.
•
Add the following line to the .cfx5rc file:
CFX_IMPORT_EXEC="<executable_path>"
where <executable_path> is the full path and name of your executable.
For details, see Resources Set in cfx5rc Files in the CFX Introduction.
•
Set CFX_IMPORT_EXEC in the system environment.
9.2. Mesh Tree View
The Mesh branch of the main tree view shows the regions of the imported meshes arranged in a hierarchy for each loaded mesh file. You can also view regions arranged in a hierarchy based on composite
regions and mesh assemblies. To view either hierarchy in a separate Mesh tree view, right-click Mesh
(from the Mesh branch of the main tree view) and select one of the View by submenu commands.
When viewing the file-based hierarchy, each imported mesh forms one or more assemblies at the first
level of the tree. The second level of the tree shows all 3D primitives and the third level shows
•
2D primitives bounding each 3D primitive
•
some composite regions.
9.2.1. Shortcut Menu Commands for Meshes and Regions
Right-clicking on a region, mesh assembly, 3D primitive, or 2D primitive in the tree view displays a
shortcut menu containing various options depending on what is selected. For details about the generic
shortcut menu commands, see Outline Tree View Shortcut Menu Commands (p. 7). Details about the
mesh-related shortcut menu items are provided in:
•
Importing Meshes (p. 65)
•
Deleting Meshes and Mesh Components from the Tree View (p. 81)
•
Transform Mesh Command (p. 82)
•
Gluing Meshes Together (p. 88)
•
Mesh Editor (p. 88)
•
Render Options (p. 88)
Note
If Highlighting
is selected (from the viewer toolbar), mesh entities will be highlighted in
the viewer when you select them in the tree view.
9.3. Deleting Meshes and Mesh Components from the Tree View
There are several options for deleting meshes and mesh components and composite regions using
shortcut menu items available in the Outline tree view in CFX-Pre. These options are:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
81
Chapter 9: Importing and Transforming Meshes
•
Delete All Mesh: Available when you right-click Mesh. When selected this option deletes all meshes
currently present.
•
Delete Mesh: Available when you right-click individual meshes themselves or Composite 3D Regions
or Primitive 3D Regions that map directly and entirely to one or more assemblies. When selected, this
option deletes all mesh associated with the selected assemblies.
•
Delete Definition: Available when you right-click a composite region. When selected this option deletes
the definition of the composite region name but not the underlying mesh.
9.4. Transform Mesh Command
You can transform meshes using the Mesh Transformation Editor dialog box. To access this dialog
box, right-click a mesh file or selection of one or more 3D meshes in the tree view, then select the
Transform Mesh command from the shortcut menu. There are four basic transformations: Rotation,
Translation, Scale, and Reflection. More complex transformations can be achieved by successive
application of the basic types. You can also copy meshes, either by retaining the original mesh, or by
creating multiple copies.
When picking points from the Viewer, the Show Faces render option must be selected to allow a point
on a region to be picked. It may also be useful to have Snap to Node selected (on by default in the
viewer toolbar).
The values entered on this form use the units defined on the Edit > Options > Common > Units form.
For details, see Units (p. 48).
The topics in this section include:
•
Target Location (p. 82)
•
Reference Coord Frame (p. 83)
•
Transformation: Rotation (p. 83)
•
Transformation: Translation (p. 84)
•
Transformation: Scale (p. 84)
•
Transformation: Reflection (p. 85)
•
Transformation: Turbo Rotation (p. 86)
•
Multiple Copies (p. 86)
•
Advanced Options (p. 87)
•
Automatic Transformation Preview (p. 88)
9.4.1. Target Location
Select the assemblies and/or other regions to transform from the Target Assemblies drop-down box.
Click the
icon to access the full list of available regions.
Not all regions are transformable. For example, 2D regions or 3D regions not resolving to at least one
assembly are not transformable.
82
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh Command
9.4.2. Reference Coord Frame
Toggle on Reference Coord Frame to specify if the transformation is defined in another coordinate
frame. Select the reference coordinate frame from the Coord Frame list.
9.4.3. Transformation: Rotation
Use the Rotation transformation to rotate an assembly about an axis defined by two points or a
principal axis.
9.4.3.1. Rotation Option: Principal Axis
This Rotation Option uses the X, Y, or Z axis as the axis of rotation. Select one of the principal axes,
under Axis, to be the axis of rotation.
9.4.3.2. Rotation Option: Rotation Axis
This Rotation Option uses a user-defined axis as the axis of rotation for the transformation. This axis
is defined by two Cartesian points, From and To. These points can be entered manually or selected in
the Viewer by clicking any coordinate box and then clicking in the Viewer.
9.4.3.3. Rotation Angle Option
The rotation angle options are Specified, Full Circle, and Two Points.
9.4.3.3.1. Specified
The Specified option simply rotates the assembly by the specified angle. When looking from the start
point to the end point of the axis, a positive angle will produce a rotation in the clockwise direction.
9.4.3.3.2. Full Circle
The Full Circle option should be used in conjunction with Multiple Copy, otherwise, the assembly will
simply be transformed back to its original position. The effect this has is described more fully in Multiple
Copy.
9.4.3.3.3. Two Points
The Two Points option calculates an angle using the axis of rotation and the two points specified, as
shown in the following figure. The two points and the start point of the axis define a plane with a
normal direction pointing towards the end point of the axis. The angle proceeds in the clockwise direction
from the Start to the End point when looking from the start point to the end point of the axis. When
picking points from the Viewer, the Show Faces render option must be selected to allow a point on a
region to be picked. It may also be useful to have Snap to Node selected (on by default in the Viewer
toolbar).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
83
Chapter 9: Importing and Transforming Meshes
9.4.4. Transformation: Translation
Use the translation transformation to move an assembly in the X, Y, and Z directions.
9.4.4.1. Method: Deltas
The Deltas method moves the mesh by the Dx, Dy, Dz values entered. Enter the Dx, Dy, Dz values
with which to translate the mesh. This is equivalent to a vector translation, using the origin as the start
point of the vector and the point entered as the end point. A point can be entered manually or selected
in the Viewer after clicking any coordinate box.
9.4.4.2. Method: Vectors
The Vector option moves the assembly by the vector described by the From and To points.
Enter From and To points to describe the translation. These points can be entered manually or selected
in the Viewer after clicking any coordinate box.
9.4.5. Transformation: Scale
The Scale method is used to scale an assembly by a scale factor.
9.4.5.1. Method: Uniform
The Uniform option uses the same scale factor for all coordinate directions, therefore scaling the size
of the assembly while maintaining the same aspect ratio. Specify the scale factor by entering a value
for Uniform Scale (which must be greater than zero).
9.4.5.2. Method: Non Uniform
The Non Uniform option can scale the assembly using a different scale factor in each coordinate
direction, producing stretching effects.
Enter a scale factor, Sx, Sy, Sz and the mesh is scaled by the scale factor value in the X, Y and Z coordinate directions.
9.4.5.3. Scale Origin
Scaling is achieved by multiplying the location of each mesh node relative to the Scale Origin by the
scaling factor.
84
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh Command
Enter the Scale Origin as a Cartesian coordinate (for example, [0 0 0]), or click any Cartesian coordinate box then pick a point from the Viewer. When you are in Picking mode, the Cartesian coordinate
boxes turn yellow. To manipulate the object in the viewer while in this state you have to click the
viewer icons (rotate, pan, zoom) in the toolbar. You can turn off Picking mode by changing the keyboard
focus (by clicking on another field, for example).
9.4.5.4. Apply Scale To
This setting controls whether the transformation is applied to the original mesh or to a copy of the
mesh. If you have set up physics locations on the original mesh, such locations are retained after the
transformation.
The following options are available:
Original (No Copy)
Transforms the original mesh without making a copy.
Copy (Keep Original)
Copies the original mesh before applying the transformation. In this case, the original mesh remains in
its current location.
9.4.6. Transformation: Reflection
The Reflection method is used to mirror a mesh in a specified plane. Apart from using the principal
planes (for example, the XY plane), arbitrary planes can be created with the Three Points and the Point
and Normal methods. These are the same plane definition methods that are available in CFD-Post.
9.4.6.1. Method
The options available are YZ Plane, XZ Plane, XY Plane, Three Points and Point and
Normal.
When using the YZ Plane, XZ Plane, or XY Plane method, an offset, X, Y, and Z respectively,
can be applied by entering a value in the X, Y, Z offset box.
If you use the Three Points or Point and Normal method, the points can be manually entered
or selected in the Viewer after you click in any coordinate field.
9.4.6.2. Apply Reflection To
This setting controls whether the transformation is applied to the original mesh or to a copy of the
mesh. If you have set up physics locations on the original mesh, such locations are retained after the
transformation.
The following options are available:
Original (No Copy)
Transforms the original mesh without making a copy.
Copy (Keep Original)
Copies the original mesh before applying the transformation. In this case, the original mesh remains in
its current location.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
85
Chapter 9: Importing and Transforming Meshes
9.4.7. Transformation: Turbo Rotation
Use the Turbo Rotation transformation to rotate an assembly about an axis defined by the rotation
axis or a principal axis.
9.4.7.1. Rotation Option: Principal Axis
This Rotation Option uses the X, Y or Z axis as the axis of rotation. Select one of the principal axis,
under Axis, to be the axis of rotation.
9.4.7.2. Rotation Option: Rotation Axis
The Rotation Option uses a user-defined axis as the axis of rotation for the transformation. This axis
is defined by two Cartesian points, From and To. These points can be entered manually or selected in
the Viewer by clicking any coordinate box and then clicking in the Viewer.
9.4.7.3. Rotation Axis Options
In addition to the From and To points, you can select the following options:
Passages per Mesh
An indication of the number of blade passages that exist in the selected mesh file. The value will normally
be 1.
Passages to Model
An optional parameter that is used to specify the number of passages in the section being modeled.
This value is used in CFD-Post.
Passages in 360
An optional parameter that is used to specify the number of passages in the machine. This value is used
in CFD-Post.
Theta Offset
Rotates the selected mesh, about the rotational axis, through an angle Theta. The offset can be a single
value or set to an expression by clicking
.
9.4.8. Multiple Copies
When the Multiple Copies toggle is disabled, then the assembly is simply transformed to the new
location, without retaining a copy of the assembly at the original location. You can enable the Multiple
Copies toggle to allow multiple copies of an assembly to be made during the transformation. It should
be noted that this section is not available for Scale Transformations.
In general, the multiple copies will be evenly spaced throughout the transformation. For rotational
transformations copies will appear at evenly spaced angles, while for translational transformations
copies will appear at evenly spaced intervals along the vector describing the translation. For example,
if you have a mesh for a single blade passage, you can make copies of it using the rotation transformation. If your full machine has 60 blades and you want to reproduce the full geometry, you should use
the Full Circle option for the Angle and select to make 59 copies (the original copy is the 60th).
9.4.8.1. # of Copies
Enter the number of copies for the assembly to make. This number does not include the original copy.
86
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh Command
9.4.8.2. Delete Original
Controls whether the original copy is retained or deleted after the transformation. Composite regions
associated with the original mesh are not deleted during this operation.
9.4.9. Advanced Options
The Advanced Options control your mesh-gluing strategy as described below.
9.4.9.1. Glue Adjacent Meshes
If you enable this toggle, CFX-Pre will attempt to automatically glue each copy of the assembly together.
This means that CFX-Pre will try to create a continuous mesh contained in a single assembly from the
multiple copies. For the glue to be successful, physically matching boundaries with one-to-one node
pairings must be found between the copy (or copies) and the original. The multiple copies will then be
treated as a single continuous mesh in a single assembly with multiple 3D regions. A single domain
can be created for the entire assembly without the need to create domain or periodic interfaces between
each copy. If multiple domains are created, automatic domain interfaces can be created. For details,
see Automatic Creation and Treatment of Domain Interfaces in the CFX-Solver Modeling Guide.
If boundaries do not physically match or one-to-one node pairings do not exist, then each copy will
form a new assembly, which will require the creation of domain interfaces to connect them together.
When Delete Original is used in conjunction with Glue Matching Meshes, the original is deleted only
if the gluing operation is successful.
For more information on gluing, see Gluing Meshes Together (p. 88).
You can set the following advanced options:
Glue Strategy
Choose the strategy that CFX-Pre will use in deciding how mesh selections being transformed are glued
with each other and with other areas of mesh:
•
Location and Transformed causes CFX-Pre to try to create connections automatically between the
selected location being transformed and any copies that are made.
•
Location and Transformed and Touching requests that CFX-Pre tries to glue the transformed
locations with any copies made and also with any other mesh locations that are in contact with the
transformed location or transformed copies.
Keep Assembly Names
An assembly is a group of mesh regions that are topologically connected. Each assembly can contain
only one mesh, but multiple assemblies are permitted.
When transforming a location, existing assemblies can be modified or created by removing connections between 3D regions or can be merged by creating connections between 3D regions. The
setting of Keep Assembly Names can be altered to indicate whether CFX-Pre should attempt to
preserve assembly names that were present in the problem before the transformation took place,
therefore ensuring that the locations used by physics objects are not invalidated:
•
None: no attempt is made by CFX-Pre to retain existing assembly names
•
Existing: assembly names specified before the transformation takes place are preserved
•
Existing and Intermediate: the names of assemblies prior to the transformation and also any intermediate assembly names created during the transformation process will be preserved.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
87
Chapter 9: Importing and Transforming Meshes
9.4.10. Automatic Transformation Preview
This toggle enables you to see the transformation before you click Apply. After you click Apply, the
preview toggle clears automatically.
9.5. Gluing Meshes Together
If there are multiple mesh assemblies that have matched meshes, you can try to glue these together
by selecting the assemblies in the tree view (using the Ctrl key), right-clicking, and selecting Glue Regions
from the shortcut menu. If the meshes match exactly, a 1:1 connection is made; otherwise a GGI connection is used. In either case, the connection appears as a mapping of two regions under Connectivity
in the tree view (for example, F3.B1.P3<->F3.B2.P4). Note that you can select Connectivity >
Hide 1:1 Connections so that the list of GGI connections is easier to work with.
Important
Merging/connecting meshes in CFX-Pre is not supported when those meshes are provided
by ANSYS Workbench during a Workbench session. Doing so may result in extra copies of
these meshes appearing when refreshing meshes.
Tip
Another way to glue two meshes together is to select Connectivity > Define Connection
from the tree view. In the Mesh Connections Editor that appears, click
to browse the
Selection Dialog for the regions to choose for Side One and Side Two. If
is selected,
the regions are highlighted in the viewer as you highlight regions in the Selection Dialog.
If a pair of meshes cannot be glued together, you can use a domain interface instead. For details, see
Domain Interfaces (p. 137).
Note
•
There is limited checking of the validity of GGI connections created by gluing meshes together.
•
When you transform or copy multiple assemblies, it is possible to have each copy glued to
its original assembly or to other copies made. For details, see Advanced Options (p. 87) in
the Transform Mesh Command (p. 82) section.
•
For more information on mesh connection types, see Mesh Connection Options in the CFXSolver Modeling Guide.
9.6. Mesh Editor
The mesh editor is described in Editing Regions in CFX-Pre (p. 96).
9.7. Render Options
The Render Options dialog box controls how 2D objects will appear in the Viewer, such as visibility,
line width, line color, and so on. Rendering for individual 2D Primitives, or any composite regions that
88
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Render Options
resolve to only one 2D Primitive, is set on the Render Options dialog box for 2D Primitives. For details,
see Render Options Dialog Box (p. 89).
Render Options for any regions that are made up of more than one 2D primitive (such as a 3D region
or a composite 2D region consisting of more than one 2D primitive) can be set on a global basis for all
2D primitives within the particular region. For details, see Render Options - Multiple 2D Regions (p. 90).
You can access the Render Options dialog box by right-clicking on a region in the tree view and then
selecting Render > Properties from the shortcut menu.
9.7.1. Render Options Dialog Box
When the Render Options dialog box is accessed by right-clicking on regions, the controls apply only
to those regions selected.
9.7.1.1. Draw Faces
Shows the faces of the mesh elements on 2D primitives. Show Faces should be selected if the effect
of changing the face options is to be seen.
9.7.1.2. Face Color
The color used for the mesh faces drawn on the 2D primitives. Pick a Face Color by clicking on the
color box to cycle through common colors or click
to select a custom face color.
9.7.1.3. Transparency
Select a Transparency level from 0 to 1, where 0 is opaque and 1 is transparent.
9.7.1.4. Draw Mode/Surface Drawing
Controls the shading property applied to mesh element faces on 2D primitives
9.7.1.4.1. Flat Shading
Each element is colored a constant color. Color interpolation is not used across or between elements.
9.7.1.4.2. Smooth Shading
Color interpolation is applied, which results in color variation across an element based on the color of
surrounding elements.
9.7.1.5. Face Culling
This controls the visibility for element faces of objects that either face the Viewer or point away from
the Viewer. Domain boundaries always have a normal vector that points out of the domain. The two
sides of a thin surface have normal vectors that point towards each other.
Note
Face Culling affects printouts performed using the Screen Capture method only.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
89
Chapter 9: Importing and Transforming Meshes
9.7.1.5.1. Front Faces
Clears visibility for all outward-facing element faces (the faces on the same side as the normal vector).
9.7.1.5.2. Back Faces
Clears visibility for inward-facing element faces (the faces on the opposite side to the normal vector).
9.7.1.5.3. No Culling
Shows element faces when viewed from either side.
9.7.1.6. Lighting
Toggle the lighting source on or off.
9.7.1.7. Specular
When selected, treats the object as a reflector of light.
9.7.1.8. Draw Lines
Shows the lines of the surface mesh elements on 2D primitives.
9.7.1.9. Edge Angle/Render Edge Angle
To change how much of the mesh wireframe is drawn, you can change the edge angle. The Edge Angle
is the angle between one edge of a mesh face and its neighboring face. Setting an Edge Angle will
define a minimum angle for drawing parts of the surface mesh. If you want to see more of the surface
mesh, reduce the edge angle.
9.7.1.10. Line Width
The line width can be changed by entering a value in the Line Width text box corresponding to the
pixel width of the line. When the box is active, the up and down arrow keys on your keyboard can be
used to increment the value.
9.7.1.11. Line Color
Pick a Line Color by clicking on the color box to cycle through common colors or click
custom line color.
to select a
9.7.1.12. Visibility
Set the visibility for the primitives in the Viewer. Clearing the visibility may improve the Viewer performance for complex meshes.
9.7.2. Render Options - Multiple 2D Regions
The Render Options dialog box for multiple regions is both an indicator of consistency of the render
options of the regions selected, and a tool to set render options for all selected regions. The presence
90
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh Topology in CFX-Pre
of a check mark in the check box for an option indicates whether consistent settings exist for that option
across all of the selected regions.
For example if the Shading option is selected and set to Flat Shading this means that all the regions
selected have their Shading options set to Flat Shading. By contrast, if Face Color is cleared this
indicates that at least one region has a different color. You can still apply a color to all regions by enabling
the check box next to Face Color and selecting a color. After any changes, CFX-Pre will recheck all objects
for consistency, and update the form accordingly. The options themselves are the same as for individual
regions.
9.8. Mesh Topology in CFX-Pre
The mesh topology in CFX-Pre is largely determined by the primitive regions imported with the mesh.
You must consider the requirements of the physics being simulated when generating the geometry
and mesh outside of CFX-Pre.
9.8.1. Assemblies, Primitive Regions, and Composite Regions
Each mesh is imported into one or more assemblies. An assembly represents a connected mesh. A mesh
containing one-to-one node connections is considered to be connected and is imported into a single
assembly.
Each assembly contains one or more 3D primitives (mesh regions), and each 3D primitive is bounded
by one or more 2D primitive mesh regions. Each 3D primitive may also contain 2D mesh primitives that
are located within the interior of the mesh. A primitive is the lowest level of region information available
in a mesh file.
Primitives could be regions that were explicitly created in the mesh generation software. However, in
some mesh files, the mesh references underlying CAD faces, in which case these will be the primitive
regions. GTM files are an example of this; a 2D primitive region will resolve to the CAD face Solid
1.2, for example. If CAD face data is available in the mesh file, then regions explicitly created in the
mesh generation software, or in CFX-Pre, will reference the CAD faces and, therefore, themselves will
not be the lowest level of region data. These regions are known as composite regions because they are
composed of one or more primitive regions.
Note
Because CFX-Pre can recognize underlying CAD surfaces from CFX GTM Files, it is not necessary
to create composite regions, although it will often make selecting locations easier in CFXPre. Other mesh types may or may not require the definition of composite regions within
CFX-Pre.
New composite regions can be created in CFX-Pre using the Regions details view. However, the topology
of the existing primitives limits the scope of composite region creation and it is not possible to create
any new primitives in CFX-Pre. For details, see Defining and Editing Composite Regions (p. 98).
The number and location of 2D primitives and 3D primitives is defined by the software that generated
the mesh. You should consider your domain, boundary condition, domain interface and subdomain
requirements when creating the mesh and create appropriate regions that can be used in CFX-Pre. You
will need to create each region explicitly in the mesh generation software if your mesh file does not
contain data that references the underlying CAD faces.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
91
Chapter 9: Importing and Transforming Meshes
If primitives reference the underlying CAD faces, it does not mean that the exact CAD geometry is recovered. The mesh simply references all the CAD faces and makes the mesh associated with them
available in CFX-Pre.
In CFX-Pre 3D primitives are always distinct, as such a mesh element is always contained in a single 3D
primitive. All regions in the mesh file that define a set of 3D elements are imported into CFX-Pre. If any
element exists in more than one grouping of elements, the import process will split the groupings so
that each element is contained within a single 3D primitive. Composite regions will be defined that
group the 3D primitives into the topology that the original mesh file represented. Depending on your
mesh file, this could include 3D subregions, solid regions, block-off regions, user defined 3D regions,
porous regions, and so on.
If a 2D primitive spans more than one 3D primitive, it will be split into multiple 2D primitives on import,
so that each 2D primitive is part of only one 3D primitive. All overlapping 2D primitives are also split
into distinct primitives upon import and composite regions are created to represent the original regions
read from the mesh file. When a 2D primitive forms a boundary between 3D primitives, it will be split
into two sides, such that a 2D primitive is associated with each 3D primitive. When a 2D primitive is
split, a suffix is added to the name so that the resulting 2D primitives are named uniquely. For example,
a 2D primitive called Solid 1.2 would be split into Solid 1.2A and Solid 1.2B.
9.8.1.1. Composite Regions
Composite regions are defined as combinations of one or more 2D primitive, 3D primitive or other
composite regions. New composite regions created in CFX-Pre must therefore be defined by a combination of at least one other region, however it is possible that a composite region can be defined that
resolves to nothing.
Composite regions that are specified in the original mesh file imported into CFX-Pre will be imported
into the application if the import format can be translated into one that CFX-Pre can use. The composite
regions imported into CFX-Pre can be selected, modified and deleted in the same way as composite
regions defined in the application.
Additional information on primitive and composite regions is available in Assemblies, Primitive Regions,
and Composite Regions (p. 91).
For details about creating regions, see Regions (p. 95).
9.8.1.1.1. Applications of the Composite Regions
For details, see Applications of Composite Regions (p. 99).
9.8.2. Domain and Subdomain Locations
Domains are created from a list of 3D primitives, and subdomains from list of 3D primitives that are
also contained in a domain. Assemblies and 3D composites can also be used as locations for domains
and subdomains. In this case, all 3D primitives contained within the assembly or 3D composite are included in the domain.
Assemblies and 3D primitives not included in a domain are not used in the simulation. A 3D primitive
may be implicitly included if it forms part of a 3D composite or assembly that is used in a domain.
The domains in a multi-domain simulation must be continuous or connected via domain interfaces you cannot have separate isolated domains.
92
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Advanced Topic: cfx5gtmconv Application
9.8.3. Boundary Condition and Domain Interface Locations
2D primitives and 2D composite regions can be used as locations to create boundary conditions and
domain interfaces.
If your assembly has more than one 3D primitive and they share a common boundary, then at least
one pair of 2D primitives will exist at the common boundary. One 2D primitive of each pair will bind
one of the 3D primitives that shares the common boundary.
It is not possible for a region to span more than one domain in a single boundary condition.
9.8.4. Importing Multi-domain Cases
Meshes intended or previously used for multi-domain simulations can be imported into CFX-Pre. You
will still be able to set up a multi-domain simulation from a single mesh import.
If the imported mesh is not connected, a separate assembly will be created for each connected section.
Each assembly can be used to create a separate domain. If the mesh is connected, then a single assembly
will be created but 3D primitives will be created for each 3D region defined in the mesh file. Each 3D
primitive can be used to create a separate domain, even if it is contained in a single assembly.
9.9. Advanced Topic: cfx5gtmconv Application
The cfx5gtmconv application is a command line executable that can be used to convert between a
number of mesh file formats. It can be used to perform import of a mesh into a GTM database or to
convert a GTM database into a CFX-Solver input file that can be viewed in CFD-Post. If appropriate
physics CCL is available, it can also be used to create a definition that can be run in a solver. In this
case, the exported mesh obeys the constraints imposed on it by the solver and the physics model.
Full details can be found by entering:
<CFXROOT>/bin/cfx5gtmconv -help
at the command line, where <CFXROOT> is the path to your installation of CFX-Pre.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
93
94
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 10: Regions
CFX-Pre has two types of regions:
•
Primitive
•
Composite
This chapter describes:
10.1. Primitive Regions
10.2. Composite Regions
10.3. Using Regions in CFX-Pre
10.4. Editing Regions in CFX-Pre
10.5. Applications of Composite Regions
Additional information on primitive and composite regions is available. For details, see Mesh Topology
in CFX-Pre (p. 91).
10.1. Primitive Regions
Primitive regions are a unique selection of 2D faces or 3D elements that define a location in the model.
A model containing a mesh will have at least one 2D primitive region and one 3D primitive region.
It is not possible for a primitive region to contain 2D faces and 3D elements.
10.2. Composite Regions
Composite regions are regions defined in terms of other regions. For example:
•
A named Region “A” may be an alias for another Region “B”
A composite region that is an alias can directly reference only one other region, but may reference
more than one region if the region it references is itself another composite region.
•
Region “C” may be a union (that is, all) of Region “D” and Region “E”.
A composite region that is a union will reference one or more other regions directly and may indirectly reference many other regions if the regions it references themselves reference other regions.
Composite regions ultimately resolve to primitive regions.
The tree view and the Region details view are used to select, create, rename, modify, and delete composite regions.
If any of the primitive regions to which a composite region resolves does not exist in the model, the
composite region is said to be unresolved.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
95
Chapter 10: Regions
Composite regions can be defined in terms of 2D and 3D primitive regions. If the composite region
resolves to both 2D and 3D primitive regions, the composite region is known as a mixed dimensionality
composite.
An Assembly is a special case of a mixed-dimensionality composite region. It can be used in the same
way, but its composition implies connectivity within the mesh. All 3D mesh volumes within an Assembly
‘know’ about their connections to each other. This information is used by CFX-Pre when calculating interfaces between domains.
Composite regions that are specified in the original mesh file imported into CFX-Pre will be imported
into the application if the import format can be translated into one that CFX-Pre can use. The composite
regions imported into CFX-Pre can be selected, modified, and deleted in the same way as composite
regions defined in CFX-Pre.
10.3. Using Regions in CFX-Pre
A composite 2D region may be used in exactly the same way as a primitive 2D region to define the
location of a Boundary Condition, Domain Interface, and so on, in the model.
A composite 3D region may be used in exactly the same way as a primitive 3D region to define the
location of a Domain or Sub-domain in the model.
Mixed-dimensionality composite regions can be used as locators, but only the primitive regions of appropriate dimensionality are used in the location. For example, a mixed-dimensionality region used as
the location of a boundary condition will mean that the boundary condition is defined only on the 2D
components.
10.4. Editing Regions in CFX-Pre
As there are two types of regions in CFX-Pre, there are two editors used for defining and modifying
these regions. For details, see:
•
Defining and Editing Primitive Regions (p. 96)
•
Defining and Editing Composite Regions (p. 98)
10.4.1. Defining and Editing Primitive Regions
Currently only definition and modification of 2D primitive regions is supported.
To define a primitive region, select Regions from the Insert > Primitive Region on the main menu or
from the shortcut menu available from Mesh in the Outline or Mesh trees. To edit an existing primitive
2D region when on the name of the region in the Outline or Mesh trees, right-click and select Edit
Mesh from the shortcut menu.
96
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Editing Regions in CFX-Pre
Faces can be moved or copied from one or more 2D primitive regions into a new or an existing 2D
primitive region.
The Region Filter enables you to modify the source from which faces will be picked. Select All Regions
from the drop-down list if faces are to be selected from anywhere in the model, or any number of regions
if you want to restrict your source regions. (Note: If you have entered the editor by selecting Edit Mesh,
the region filter will be set to the regions selected in the tree by default. You are able to change this
selection if required.)
Initially no faces will be selected in the viewer and the dialog box will indicate this.
Click Start Picking and use one of the toolbar buttons on the 3D viewer, for details, see 3D Viewer
Toolbar (p. 19):
•
To set the pick mode to single face selection, click this button. Clicking in the viewer will select
the first face to move.
•
To flood fill an area, click this button and then click in the viewer. Changing the crease angle will
control how far the flood will extend. The angle indicates that any face that bounds the face first selected
and has a normal within the angle will be selected. The same angle is then used again on any faces
selected by the algorithm until no more faces can be reached using this method.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
97
Chapter 10: Regions
•
To select all faces within a rectangle, click this button and then click in the viewer and drag the
box to perform the selection. The option to the left of Pick All indicates whether the selection only includes fully enclosed faces or any touching or enclosed faces.
•
To select all faces within a polygon, click this button and then click multiple times in the viewer
finishing with a double-click to perform the selection. The option to the left of Pick All indicates
whether the selection only includes fully enclosed faces or any touching or enclosed faces.
Appending further faces to the current selection is performed in the same way as above, but by using
Ctrl and click to pick the faces in the viewer. All operations can use this method.
The names of the 2D primitive regions from which faces have been selected are shown in the Mesh
Face Selection tree. The number of faces selected from each 2D primitive is also shown. The set of
faces associated with a single 2D primitive can be removed by right-clicking the 2D primitive in the
tree.
Faces are moved or copied to a destination region; the action can be selected from those shown in
Destination box.
You can select the destination for the faces from the list to the right of the Move Faces To field, or you
can type a new name into the field.
Note
Unexpected results may occur if the topology of the current model is altered in some way
during the course of the edit. For example adding a new composite region or deleting an
existing one or importing or deleting a mesh may alter how the editor acts. In a similar way,
performing an Undo or Redo when faces are selected may change the topology. If any of
these operations are performed, click Reset and re-pick the faces as required.
10.4.1.1. Advanced Options
At the bottom of the form, the Options box can be expanded and Remove Invalid Components from
Composite Definitions can be selected. Selecting this option will remove any references to primitives
that are completely removed by the operation. If this is not done, composite regions that reference a
removed primitive region will become unresolved.
10.4.2. Defining and Editing Composite Regions
The Regions details view is used to create new, and edit existing composite regions. To create a new
region, select Composite Region from either the Insert >Regions menu or the shortcut menu available
from Mesh in the Outline or Mesh trees. To edit an existing composite region, right-click it in the Outline
or Mesh tree view, then select Edit Definition from the shortcut menu.
A composite region is defined by specifying a list of regions and a method for combining them. The
Regions details view can be used to create or modify a region by selecting a method of combination
from the Combination list and a selection of regions from the Region List.
98
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Applications of Composite Regions
Note
The Regions details view enables you to restrict the regions available for selection by limiting
them by Dimension(Filter). Selecting 2D will cause the Region List to only display 2D regions
and selecting 3D will cause the Region List to only select 3D regions. Regions of mixed dimensionality are always available.
10.4.2.1. Union
A Combination setting of Union combines the area or volume of the selected regions to create a new
region. The new region will include all the regions from which it is constructed. For example, two or
more 3D regions can be combined to create a new region, which can then be used as the location for
a domain.
10.4.2.2. Alias
A Combination setting of Alias is used to produce a composite region that when resolved is based
upon the same set of primitive regions as the region it is defined on. A composite region with a Combination of Alias may only reference a single region (this may be a composite or primitive region).
The new composite region may, however, resolve to more than one primitive region. This feature is
useful to assign recognizable names to regions with non-intuitive names.
10.5. Applications of Composite Regions
Composite Regions that are defined in the simulation can be used as locations for domains, sub-domains,
boundary conditions and domain interfaces. For example, a composite region with a combination
method of Union can be used to group two separate 3D regions. A domain that spans both 3D regions
can then be created using the single composite 3D region. Domain interfaces should still be created
to connect the two assemblies together if the composite region does not form a continuous mesh and
flow is to pass between the two assemblies. For details, see Mesh Topology in CFX-Pre (p. 91).
Another application of composite regions is to set up a consistent set of locations that can be applied
to a number of different simulations that use the same physics definition. By referencing the composite
regions in the physics definitions, the need to edit the definitions for each mesh is avoided and if differences in the mesh topology do exist this can be coped with by editing the composite regions used
to locate the physics relatively simply. In this way for every problem in which the physics is to be applied,
the mesh, region CCL, and physics CCL can be imported. Locations of boundary conditions, domains
and subdomains should all match provided that the composite regions can all be resolved as expected.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
99
100
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 11: Analysis Type
The Analysis Type details view is used to specify whether the analysis requires coupling to an external
solver, such as ANSYS Multi-field, and whether the analysis is steady state, transient, or transient blade
row. A discussion of external solver coupling is presented in Coupling CFX to an External Solver: ANSYS
Multi-field Simulations in the CFX-Solver Modeling Guide. A discussion on steady state and transient flows
is presented in Steady State and Transient Flows in the CFX-Solver Modeling Guide.
11.1. Basic Settings Tab
The following topics are discussed in this section:
•
External Solver Coupling Settings (p. 101)
•
Analysis Type Settings (p. 101)
11.1.1. External Solver Coupling Settings
Most analyses will require no coupling to another solver and Option can remain set to the default of
None. If you are setting up a two-way fluid-structure analysis, coupling CFX-Solver to ANSYS solver,
then you need to set Option to either ANSYS MultiField or ANSYS MultiField via Prep7.
Use ANSYS MultiField if you want to do a full ANSYS Multi-field set-up, or ANSYS MultiField
via Prep7 if you want to do a minimal set-up in CFX-Pre and define the ANSYS Multi-field set-up in
the ANSYS Prep7 user interface. A full description of these two modes of operation can be found in
Overview of Pre-Processing for ANSYS Multi-field Simulations in the CFX-Solver Modeling Guide.
If ANSYS MultiField is selected, then additional information must be specified. The ANSYS Input
File setting is described in Input File Specification for the Mechanical Application in the CFX-Solver
Modeling Guide, and the Coupling Time Control settings are described in Coupling Time Control in
the CFX-Solver Modeling Guide.
11.1.2. Analysis Type Settings
The Analysis Type settings enable you to specify an analysis as being Steady State, Transient,
or Transient Blade Row. Steady state analyses are used to model flows that do not change over
time; transient analyses model flows that are time-dependent. Transient blade row analyses are transient
analyses that have special handling for turbomachinery cases.
The Analysis Type options are described in the following sections:
•
Steady State (p. 102)
•
Transient (p. 102)
•
Transient Blade Row (p. 103)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
101
Chapter 11: Analysis Type
11.1.2.1. Steady State
No further settings are required for the Steady State option. Modeling advice for setting the time
scale for steady state simulations is provided in Steady State Time Scale Control in the CFX-Solver Modeling Guide.
11.1.2.2. Transient
11.1.2.2.1. Time Duration
Set Option to determine the length of the transient analysis:
•
Total Time
•
Time per run
•
Maximum Number of Timesteps
•
Number of Timesteps per Run
•
Coupling Time Duration
For details, see Time Duration in the CFX-Solver Modeling Guide.
11.1.2.2.2. Time Steps
Set Option to determine the size of timesteps for the run:
•
Timesteps
•
Timesteps for the Run
•
Adaptive
•
Coupling Timesteps
The Timesteps and Timesteps for the Run parameters can accept a single value or lists. If a list is
entered, it should be comma separated, for example, 2, 1.2, 2.4. If an expression is used, you must
associate units with each item in the list, for example, 2 [s], 1.2 [s], 2.4 [s]. In addition, it
is possible to define multiples of a timestep value in the user interface when not using the expression
method. For example, you could enter 5*0.1, 2*0.5, 10*1 as a list of values, and set the units to
[s] separately. The corresponding CCL that would be generated would be:
0.1 [s], 0.1 [s], 0.1 [s], 0.1 [s], 0.1 [s], 0.5 [s], 0.5 [s], 1 [s],
1 [s], 1 [s], 1 [s], 1 [s], 1 [s], 1 [s], 1 [s], 1 [s], 1 [s]
If you accidentally enter 5*0.1 [s], 2*0.5 [s], 10*1 [s] as an expression, the multiplication
would be carried out, and the corresponding CCL that would be generated would be:
0.5 [s], 1.0 [s], 10.0 [s]
For details, see Transient Timestep Control in the CFX-Solver Modeling Guide.
When Adaptive time is selected, set one of the following three conditions for Timestep Adaption
to automate the calculation of timestep size:
•
Number of Coefficient Loops
•
RMS Courant Number
102
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Basic Settings Tab
•
MAX Courant Number
For details, see Transient Timestep Control in the CFX-Solver Modeling Guide.
11.1.2.2.3. Initial Time
Set the Option to specify the Initial Time for a transient analysis.
•
Automatic
•
Automatic with Value
•
Value
•
Coupling Initial Time
For details, see Initial Time in the CFX-Solver Modeling Guide.
11.1.2.3. Transient Blade Row
The Transient Blade Row option is required in order to access the Transient Blade Row models:
•
None
•
Profile Transformation
•
Time Transformation
•
Fourier Transformation
The Initial Time settings must be specified in the Analysis Type settings. For details on these settings,
see Initial Time (p. 103).
For instructions on setting up and using Transient Blade Row models, see Transient Blade Row Modeling
in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
103
104
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 12: Domains
This chapter describes:
12.1. Creating New Domains
12.2.The Details View for Domain Objects
12.3. Using Multiple Domains
12.4. User Interface
CFX-Pre uses the concept of domains to define the type, properties, and region of the fluid, porous, or
solid. Domains are regions of space in which the equations of fluid flow or heat transfer are solved. This
section describes how to use the domain details view to define the physics of fluid, porous or solid
domains in your simulation. This includes selecting the 3D bounding regions and choosing appropriate
physical models.
A list of the physical models available in CFX, as well as additional information on the physical meaning
of the models used, is available. For details, see Physical Models in the CFX-Solver Modeling Guide.
Domains are created from a list of Assemblies, 3D primitive regions and/or 3D composite regions that
are associated with a volume of an imported mesh. A discussion of these objects can be found in CFXPre. For details, see Mesh Topology in CFX-Pre (p. 91).
In some cases, separate domains will need to be connected via a domain interface, while in other cases,
no interface is required or a default interface is created and is suitable. For details, see Domain Interfaces (p. 137).
Within fluid, porous, and solid domains, internal 3D regions can be assigned to a subdomain. These are
used to create volumetric sources of mass, momentum, energy, and so on. For details, see Subdomains (p. 181).
Boundary conditions can be applied to any bounding surface of a 3D primitive that is included in a
domain (that is, including internal surfaces). For details, see Boundary Conditions (p. 149).
12.1. Creating New Domains
New domains are created by selecting Insert > Domain or clicking the Domains
icon. Note that
creation of domains from the menu bar or toolbar may subsequently require selection of the appropriate
analysis type. Domains can also be created by right-clicking the appropriate analysis type in the Outline
view.
Creating a new domain will present a dialog box where a unique name for the domain should be
entered.
Additional information on valid names is available in Valid Syntax for Named Objects (p. 55). Existing
domains may be edited by double-clicking the domain in the Outline view, or by right-clicking the
domain and selecting Edit. For details, see Outline Tree View (p. 5).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
105
Chapter 12: Domains
12.2. The Details View for Domain Objects
After entering a name for the domain, or selecting a domain to edit, the domain details view appears
in the workspace. In this view, you should complete each of the following tabs in turn, proceeding from
left to right across the tabs. The tabs shown depends on your simulation, but could be:
•
Basic Settings: Sets the location and type of domains, as well as the fluid, porous or solid, used in the
domain. The reference pressure, buoyancy options and domain motion are also set here. For details,
see Basic Settings Tab (p. 107).
•
Porosity Settings: Only available for porous domains. Set the general description of a porous domain.
•
Fluid Models: Only available for fluid domains. Sets the physical models that apply to all domain fluids.
For details, see Fluid Models Tab (p. 113).
•
Fluid Specific Models (for example, Water at RTP): Only available for fluid or porous domains when
more than one fluid is selected, or for a single phase case when particles are included. A separate tab
is used for each fluid in the domain and uses the fluid name as the name for the tab. This sets physical
model options that are specific to each domain fluid. For details, see Fluid Specific Models Tab (p. 119).
•
Fluid Pair Models: Only available for fluid domains using multiple fluids or when particles are included.
This sets options that depend on the interaction between fluid pairs, such as transfer options. For details,
see Fluid Pair Models Tab (p. 122).
•
Solid Models: Only available for solid domains. Sets the physical models that apply to the solid. For
details, see Solid Models Tab (p. 128).
•
Particle Injection Regions: When a particle tracking simulation is used, custom injection regions can
be created using this tab. For details, see Particle Injection Regions Tab (p. 131).
•
Initialization: Sets initial conditions on a domain basis. For details, see Initialization Tab (p. 135). This is
optional since global initialization can also be performed, but is essential for solid domains.
•
Solver Control: Sets solver control settings on a domain basis. For details, see Solver Control Tab (p. 135).
12.3. Using Multiple Domains
For any given CFD problem, more than one domain may be defined. By default, the physical models
used in each domain must be consistent; therefore, each time you create or edit a domain, the physical
models (fluid lists, heat transfer models, and so on) are applied across all domains of the same type
(such as fluid or solid), possibly overwriting models chosen earlier for other domains.
Note the following:
•
Some exceptions exist when using fluid and solid domains together and also to allow MFR (multiple
frame of reference) simulations to be defined.
•
If a domain interface is required, refer to Using Domain Interfaces in the CFX-Solver Modeling Guide for
information on the correct use of interfaces.
12.3.1. Multiple Fluid Domains
When consistent physics has been enforced, all settings are copied across all fluid domains when any
fluid domain is edited with the following exceptions:
•
Location: The location of each domain must obviously be different.
•
Coordinate Frame: Each domain can use a different reference local coordinate frame.
106
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
•
Domain Motion: Each domain can be independently stationary or rotating. For rotating domains, the
angular velocity and axis of rotating can be different for each domain. This enables MFR simulations to
be set up.
Note that these parameters are all set on the Basic Settings tab on the Domains form.
Fluid and Solid Domains: Settings are not copied between fluid and solid domains with the exception
of Thermal Radiation Model. If any solid domain uses the Monte Carlo radiation model, then all fluid
domains must also model radiation and must use the Monte Carlo model. If no solid domain has radiation
modeling (that is, Option = None), then the fluid domains can use any radiation model.
12.3.2. Multiple Solid Domains
Settings are not copied between solid domains. Each solid domain can be made from a different material and can mix the Monte Carlo radiation model and no radiation model.
12.4. User Interface
The following topics will be discussed:
12.4.1. Basic Settings Tab
12.4.2. Fluid Models Tab
12.4.3. Polydispersed Fluid Tab
12.4.4. Fluid Specific Models Tab
12.4.5. Fluid Pair Models Tab
12.4.6. Solid Models Tab
12.4.7. Porosity Settings Tab
12.4.8. Particle Injection Regions Tab
12.4.9. Initialization Tab
12.4.10. Solver Control Tab
12.4.1. Basic Settings Tab
The basic settings apply to the whole of the domain. When you create a new domain, the Basic Settings
tab is initially shown.
12.4.1.1. Location and Type
12.4.1.1.1. Location
The Location is the list of assemblies, 3D primitive regions and/or 3D composite regions that define
the volume of the domain. For details, see Mesh Topology in CFX-Pre (p. 91). Using an assembly or a
composite region in the Location list implicitly includes all 3D primitives contained within the object.
You can use more than one location by using the Shift or Ctrl keys to pick multiple entries from the
drop-down list. The
icon to the right of the drop-down list can be used to pick locations from an
expanded list. Alternatively, clicking a location in the viewer displays a small box containing the available
locations.
For details, see Domain and Subdomain Locations (p. 92).
12.4.1.1.2. Domain Type
The Domain Type setting can be set to one of the following:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
107
Chapter 12: Domains
•
Fluid Domain
Fluid domains are used to model one fluid or a combination of fluids, with a wide range of modeling
options. It is possible to deform the mesh to simulate movement of the boundaries of the domain;
for details, see Mesh Deformation (p. 113).
•
Solid Domain
Solid domains are used to model regions that contain no fluid or porous flow. Several modeling
options are available, including heat transfer (see Conjugate Heat Transfer in the CFX-Solver Modeling
Guide), radiation (see Radiation Modeling in the CFX-Solver Modeling Guide), and Additional Variables
(see Additional Variables (p. 275) and Additional Variables in the CFX-Solver Modeling Guide). In addition, you can model the motion of a solid that moves relative to its reference frame; for details,
see Solid Motion (p. 128).
•
Porous Domain
Porous domains are similar to fluid domains, but are used to model flows where the geometry is
too complex to resolve with a grid. For details, see Flow in Porous Media in the CFX-Solver Theory
Guide.
•
Immersed Solid
Immersed Solid domains can be used in transient simulations to model rigid solid objects that
move through fluid domains; for details, see Domain Motion (p. 111) and Immersed Solids in the
CFX-Solver Modeling Guide.
12.4.1.1.3. Coordinate Frame
By default in a fluid domain, Coordinate Frame is set to the default Cartesian frame, Coord 0, but
you can select any predefined coordinate frame. To create a new coordinate frame, select Insert > Coordinate Frame from the menu bar. For details, see Coordinate Frames (p. 255) and Coordinate Frames
in the CFX-Solver Modeling Guide.
The coordinate frame set for a domain is local to only that domain and is used to interpret all x, y and
z component values set in the domain details view. This includes the gravity components in a buoyant
flow and the rotation axis definition in a rotating domain. The coordinate frame set here has no influence
on boundary conditions for the domain. For details, see Global Coordinate Frame (Coord 0) in the CFXSolver Modeling Guide.
12.4.1.2. Fluid and Particle Definitions and Solid Definitions
To define a fluid, particle or solid (including the solid portion of a porous domain):
1.
If required, click Add new item
to the right of the definition list, type a name for the definition and
click OK. For multiphase simulation, more than one fluid is required. For details, see Multiphase Flow
Modeling in the CFX-Solver Modeling Guide.
2.
For the definition Option select Material Library (the default) to enable choosing a material
from a supplied or user defined library or Material Definition for Reacting Mixtures.
3.
For the definition Material select from the drop-down list for some commonly used materials or click
Select from extended list
108
to access a complete list of materials.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
4.
After clicking
you may also choose to select Import Library Data
to load library data from a
file.
The specification of material properties (for example, density and viscosity) and the creation of custom
materials is performed in the Materials details view. For details, see Materials (p. 259). New materials
are added to the relevant drop-down list.
A solid domain must be made from a single solid material.
12.4.1.2.1. Morphology
Which morphology options are available depends on whether you are setting fluid-specific details for
an Eulerian phase or for a particle phase. For Eulerian phases, the options are:
•
Continuous Fluid
•
Dispersed Fluid
•
Dispersed Solid
•
Droplets with Phase Change
•
Polydispersed Fluid
For details, see Morphology in the CFX-Solver Modeling Guide.
For a particle phase, the options are:
•
Particle Transport Fluid
•
Particle Transport Solid
For details, see Particle Morphology Options in the CFX-Solver Modeling Guide.
12.4.1.2.1.1. Mean Diameter
For Dispersed Fluid and Dispersed Solid phases, a mean diameter is required. For details,
see Mean Diameter in the CFX-Solver Modeling Guide.
12.4.1.2.1.2. Minimum Volume Fraction
This is available for dispersed phases, but you will not usually need to set a value. For details, see Minimum Volume Fraction in the CFX-Solver Modeling Guide.
12.4.1.2.1.3. Maximum Packing
This is available for the Dispersed Fluid and Dispersed Solid phases. For details, see Maximum
Packing in the CFX-Solver Modeling Guide.
12.4.1.2.1.4. Restitution Coefficient
This restitution coefficient setting holds a value from 0 to 1 that indicates the degree of elasticity of a
collision between a pair of particles. For such a collision, the restitution coefficient is the ratio of separation speed to closing speed. This restitution coefficient setting is used only for the kinetic theory
model. For details, see Kinetic Theory Models for Solids Pressure in the CFX-Solver Theory Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
109
Chapter 12: Domains
12.4.1.2.1.5. Particle Diameter Distribution
This is available for particle phases. For details, see Particle Diameter Distribution in the CFX-Solver
Modeling Guide.
12.4.1.2.1.6. Particle Shape Factors
This is available for particle phases. For details, see Particle Shape Factors in the CFX-Solver Modeling
Guide.
12.4.1.2.1.7. Particle Diameter Change
This option is available when multiphase reactions have been enabled with particle tracking. When
Particle Diameter Change is selected choose either Mass Equivalent or Swelling Model.
12.4.1.2.1.7.1. Swelling Model
Select a reference material from the list. Enter a Swelling Factor greater than or equal to zero; a value
of zero indicates no swelling, and CEL expressions are permitted. For details, see Particle Diameter
Change Due to Swelling in the CFX-Solver Modeling Guide.
12.4.1.3. Particle Tracking
To include particles in the domain, define a particle in Fluid and Particle Definitions..., select the
particle material and select the Particle Transport Fluid or Particle Transport Solid option for Fluid
and Particle Definitions... > <particle definition> > Morphology on the Basic Settings tab. For details,
see Particle Transport Modeling in the CFX-Solver Modeling Guide.
12.4.1.4. Domain Models
12.4.1.4.1. Pressure: Reference Pressure
This sets the absolute pressure level to which all other relative pressure set in a simulation are measured.
For details, see Setting a Reference Pressure in the CFX-Solver Modeling Guide.
12.4.1.4.2. Buoyancy: Option
For flows in which gravity is important, you should include the buoyancy term. Gravity components in
the x, y and z directions should be entered; these are interpreted in the coordinate frame for the domain.
For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
There are two different buoyancy models in CFX: the one used depends upon the properties of the
selected fluid(s). Depending on the types of fluid selected, a Buoyancy Reference Temperature and
/ or a Buoyancy Reference Density must be set. This is because different fluids use either the full or
Boussinesq buoyancy model. In multiphase flows, the reference density can have a significant effect.
The Buoyancy Reference Location can be set automatically, or to a specific location with X/Y/Z coordinates. For details, see:
•
Buoyancy in the CFX-Solver Modeling Guide
•
Buoyancy in the CFX-Solver Theory Guide.
110
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
12.4.1.4.3. Domain Motion
The available Domain Motion options depend on the type of domain, and are described in
Table 12.1: Domain Motion Options (p. 111):
Table 12.1 Domain Motion Options
Option
Eligible Domain
Types
Description
Stationary
All domain types
The domain remains stationary in the absolute frame
of reference.
Rotating
All domain types
The domain rotates with a specified angular velocity
about the given axis.
For fluid, porous, and solid domains, a Rotational
Offset setting exists.
For fluid and porous domains, an Alternate Rotation
Model option exists.
Speed
and Direction
Immersed solid domain
The domain translates at the specified speed in the
specified direction. The translation direction can be
specified by Cartesian components, or by a coordinate
axis.
Specified
Displacement
Immersed solid domain
The domain is displaced according to the specified
Cartesian components. For example, you could use CEL
expressions that are functions of time to move the
domain.
General
Motion
Immersed solid domain
Specify a reference origin that is considered to be attached to the domain. Then specify a motion for that
origin, and a rotation of the domain about that origin.
The reference origin location is specified by the Reference Location settings.
The motion of the reference origin is specified by Origin Motion settings that are similar to those for the
Domain Motion options (other than General Motion).
The rotation of the domain about the reference origin
is specified by the Body Rotation settings.
Rigid
Body Solution
Immersed solid domain
Specify a mass, moment of inertia, and various dynamics settings. The dynamics settings include external
forces and torques, translational and rotational degrees
of freedom, and gravity. All of these settings are analogous to the settings of the rigid body object, which
is described in Rigid Bodies (p. 187). Note that, unlike
for a rigid body object, you cannot specify initialization
values for the rigid body solution that applies to an
immersed solid domain; these initialization values (such
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
111
Chapter 12: Domains
Option
Eligible Domain
Types
Description
as angular velocity and angular acceleration) are effectively initialized with values of magnitude zero.
For additional information on modeling rigid bodies,
see Rigid Body Modeling in the CFX-Solver Modeling
Guide.
Details of some of the settings mentioned in Table 12.1: Domain Motion Options (p. 111):
•
Angular Velocity: The angular velocity gives the rotation rate of the domain, which can be a function
of time.
•
Axis Definition: The axis of rotation can be a coordinate axis of the local coordinate frame or a local
cylindrical axis defined by two points.
–
If Coordinate Axis is selected, the available axes are all local and global coordinate axes. Coord
0 is the global coordinate frame, and its axes are referred to as Global X, Global Y and Global Z. A local coordinate frame's axes are referred to as myCoord.1, myCoord.2, myCoord.3
where 1,2,3 represent the local X,Y,Z directions.
–
If Two Points is selected, Rotation Axis From and Rotation Axis To must be set. The points are
interpreted in the coordinate frame for the domain. If the coordinate frame is cylindrical, then the
components correspond to the r, , z directions. For details, see Coordinate Frames in the CFX-Solver
Modeling Guide.
•
Rotational Offset: This setting transforms the domain by the specified rotation angle. The rotation axis
used for this transformation is specified by the Axis Definition settings.
•
Alternate Rotation Model: For details, see Alternate Rotation Model in the CFX-Solver Modeling Guide.
•
Reference Location: The reference location is an origin point that should be defined to conveniently
describe the body rotation of the immersed solid domain. When Body Rotation > Option is set to
None, the reference location will be neglected. Specify the reference location by choosing an existing
coordinate frame origin, or by specifying Cartesian coordinates.
A solver run that starts from a previous run should have the same domain motion options in the
immersed solids domains, and must have identical reference location specifications if supplied.
•
Origin Motion: The origin motion can be specified in any of the ways that the domain motion can be
specified (not counting the General Motion option for domain motion), and by Specified Velocity, which accepts Cartesian components of velocity.
•
Body Rotation: The body rotation options are:
–
None
–
Rotating
Specify an angular velocity and the instantaneous axis of rotation.
–
Specified Angular Velocity
Use Cartesian components to define a vector. The rotation axis passes through the reference
location in the direction of the specified vector. The angular velocity is the magnitude of the
specified vector.
112
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
Note
•
CEL expressions used to define domain motion can be functions of time only.
•
If you create two or more fluid domains and modify a model setting of one of the domains,
that setting is generally copied to all other fluid domains in the simulation. An exception to
this is that if you edit the Domain Motion settings of a domain, those settings are not copied
to any other domains; this enables each domain to rotate or remain stationary independently
of the other domains.
12.4.1.4.4. Mesh Deformation
Mesh deformation can be used to model flows with a varying geometry, for both transient and steadystate simulations. There are three options for the specification of mesh deformation for a domain:
•
None
•
Regions of Motion Specified: permits wall boundaries and subdomains to move, and makes
mesh motion settings available. These include a mesh motion option (which must be set to Displacement Diffusion) and mesh stiffness settings. For details, see Regions of Motion Specified in the
CFX-Solver Modeling Guide.
•
Junction Box Routine: reads mesh coordinate datasets from a file into the CFX-Solver as the
solution proceeds. This step requires the specification of a series of meshes and User Fortran routine(s).
For details, see Junction Box Routine in the CFX-Solver Modeling Guide.
12.4.1.4.5. Passage Definition
For Transient Blade Row cases, specify the number of passages in 360° and the number of passages
per component for the domain. This information may be used in the automatic calculation of time step
size, depending on the Transient Details settings (which are described in Transient Details (p. 242)).
12.4.2. Fluid Models Tab
The Fluid Models tab is where models are chosen, which apply to all Eulerian fluids in the simulation.
By default, the fluids models must be consistent between all fluid domains in a multidomain simulation,
but CFX supports inconsistent physics through the setting of an environment variable. For details, see:
•
Using Multiple Domains (p. 106)
•
Solid Models Tab (p. 128).
In a multiphase simulation, the options that are allowed to vary between fluids will appear on the Fluid
Specific Models tab instead. For details, see Fluid Specific Models Tab (p. 119).
Some fluid models can apply to all fluids or can be set on a fluid-specific basis, these models will appear
on the Fluid Models section with a Fluid Dependent option. If this is selected, then the model
appears on the Fluid Specific Models tab.
The options available on the Fluid Specific Models tab depends on the simulation set up (including
the type and number of fluids used in the simulation (such as single or multicomponent, single or
multiphase, reacting or non-reacting)) and whether Additional Variables have been created.
All details related to Particle Tracking are set on the General Settings tab and the models chosen on
the Fluid Models tab do not apply to the particle phase.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
113
Chapter 12: Domains
Radiation with multiphase is not supported. However, it is allowed for single Eulerian particle tracking
cases on the Fluid Specific Models tab.
The available settings depend on the physical models chosen in your simulation.
12.4.2.1. Multiphase Options
These options are only applicable to multiphase simulations.
12.4.2.1.1. Homogeneous Model
Inhomogeneous is the general case of multiphase flow, where each fluid has its own velocity field,
turbulence field, and so on. You can select the Homogeneous Model check box to switch to this
model, where all fluids share a velocity field, turbulence field, and so on. For details, see The Homogeneous and Inhomogeneous Models in the CFX-Solver Modeling Guide. Both the inhomogeneous and homogeneous models have a Free Surface Model option.
12.4.2.1.2. Free Surface Model
You can select the Standard free surface model if you are modeling multiphase flow with a distinct
interface between the fluids. For details, see Free Surface Flow in the CFX-Solver Modeling Guide.
12.4.2.1.3. Multiphase Reactions
Multiphase Reactions are available when any reactions have been defined with type Multiphase. For
details, see Multiphase: Basic Settings (p. 272). Any reactions that are to be included in the simulation
should be selected from the drop-down list. For details, see Multiphase Reactions in the CFX-Solver
Modeling Guide.
12.4.2.2. Heat Transfer
12.4.2.2.1. Homogeneous Model
For details, see Homogeneous Heat Transfer in Multiphase Flow in the CFX-Solver Modeling Guide.
12.4.2.2.2. Heat Transfer: Option
Depending on your simulation, the following heat transfer options are possible. For details, see Heat
Transfer in the CFX-Solver Modeling Guide.
•
None: Not available for compressible fluids, since a temperature is required at which to evaluate the
fluid properties.
•
Isothermal: Not available for reacting fluids.
•
Thermal Energy: Models the transport of enthalpy through the fluid and is suitable for modeling
heat transfer in low-speed flows. For details, see The Thermal Energy Equation in the CFX-Solver Theory
Guide.
The Turbulent Prandtl Number may be customized by selecting the Turbulent Flux Closure
check box in the Turbulence settings.
•
114
Total Energy: Includes high-speed energy effects. You can include the Viscous Work Term in the
energy equation. For details, see The Total Energy Equation in the CFX-Solver Theory Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
The Turbulent Prandtl Number may be customized by selecting the Turbulent Flux Closure
check box in the Turbulence settings.
•
Fluid Dependent: Is used to set different heat transfer models for each fluid in a multiphase simulation. A heat transfer model is then set for each fluid on the Fluid Specific Models tab. This option
cannot be used when Homogeneous Model is selected.
12.4.2.3. Turbulence
Advice on which turbulence model is appropriate for your simulation and a description of each model
can be reviewed. For details, see:
•
Turbulence and Near-Wall Modeling in the CFX-Solver Modeling Guide
•
Turbulence Modeling in Multiphase Flow in the CFX-Solver Modeling Guide
•
Turbulence Models in the CFX-Solver Theory Guide.
12.4.2.3.1. Homogeneous Model
If you have not selected Homogeneous Model under Multiphase Options, then Homogeneous
Model under Turbulence frame will be available.
If selected, this will solve a single turbulence field for an inhomogeneous simulation. There will be no
fluid-specific turbulence data to set. For details, see Homogeneous Turbulence in Inhomogeneous Flow
in the CFX-Solver Modeling Guide.
If you do not enable this check box, then you will usually select Fluid Dependent and specify turbulence data on the fluid-specific tabs. Alternatively, the Laminar model can be picked to apply to all
fluids (this is not homogeneous turbulence).
Homogeneous multiphase flow always uses homogeneous turbulence; therefore, you only need select
the turbulence model to use.
12.4.2.3.2. Turbulence: Option
You can select one of the following turbulence models:
•
None (Laminar): Turbulence is not modeled. This should only be used for laminar flow. Of the
combustion models, only Finite Rate Chemistry is available for laminar flow. For details, see The Laminar
Model in the CFX-Solver Modeling Guide.
•
k-Epsilon: A standard fluid model that is suitable for a wide range of simulations. For details, see
The k-epsilon Model in the CFX-Solver Modeling Guide.
•
Fluid Dependent: Allows you to set different turbulence models for each fluid in the domain. If this
option is selected, the turbulence model for each fluid is set in the Fluid Specific Models tab. This is
only available for multiphase simulations when Homogeneous Model is not selected.
•
Shear Stress Transport: Recommended for accurate boundary layer simulations. For details,
see The k-omega and SST Models in the CFX-Solver Modeling Guide.
•
Omega Reynolds Stress / BSL Reynolds Stress: For details, see Omega-Based Reynolds
Stress Models in the CFX-Solver Modeling Guide.
•
QI / SSG / LRR Reynolds Stress: Provides high accuracy for some complex flows. For details,
see Reynolds Stress Turbulence Models in the CFX-Solver Theory Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
115
Chapter 12: Domains
•
Zero Equation: Only the Finite Rate Chemistry combustion model is available when using the zero
equation turbulence model. For details, see The Zero Equation Model in the CFX-Solver Modeling Guide.
•
RNG k-Epsilon: A variation of the k-epsilon model.
•
k-Omega / BSL: The SST model is often preferred to this model.
•
k epsilon EARSM / BSL EARSM: These models are a simplified version of the Reynolds Stress
models with application to problems with secondary flows as well as flows with streamline curvature
and/or system rotation. For details, see Explicit Algebraic Reynolds Stress Model in the CFX-Solver Theory
Guide
•
LES Smagorinsky / LES WALE / LES Dynamic Model: Available for transient simulation
only. For details, see The Large Eddy Simulation Model (LES) in the CFX-Solver Modeling Guide.
•
Detached Eddy Simulation: Available for transient simulation only. For details, see The Detached
Eddy Simulation Model (DES) in the CFX-Solver Modeling Guide.
The available Advanced Turbulence Control settings for turbulence modeling depend on the turbulence
model. The settings can be used to specify the coefficients for the selected turbulence model. For details,
refer to the appropriate sections of the Turbulence and Near-Wall Modeling in the CFX-Solver Modeling
Guide and Turbulence and Wall Function Theory in the CFX-Solver Theory Guide.
12.4.2.3.3. Buoyancy Turbulence
Buoyancy Turbulence is available for two (or more) equation turbulence models. For details, see Buoyancy
Turbulence in the CFX-Solver Modeling Guide.
12.4.2.3.4. Wall Function
The wall function is automatically set depending on the turbulence model selected. Therefore, you will
not need to change this setting. For multiphase flow, if the fluid dependent turbulence model option
is selected, the wall function option appears on the fluid- specific tabs. The Laminar and zero equation
turbulence models do not use wall functions. For details, see Modeling Flow Near the Wall in the CFXSolver Modeling Guide.
12.4.2.3.5. Turbulent Flux Closure for Heat Transfer
Turbulent Flux Closure for Heat Transfer is available for turbulent flow with Thermal Energy or Total
Energy heat transfer model. For details, see Heat Transfer in the CFX-Solver Modeling Guide.
12.4.2.4. Reaction or Combustion Model
If the fluid material is defined as Option is Material Definition and Composition Option is
Reacting Mixture, or if a reacting mixture from the material library has been selected as the material for one of the domain fluids, then you can select a combustion model as:
•
Eddy Dissipation
•
Finite Rate Chemistry
•
Finite Rate Chemistry and Eddy Dissipation
•
PDF Flamelet
•
BVM (Partially Premixed)
•
Extended Coherent Flame Model
•
Fluid Dependent (multiphase only)
116
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
Only Finite Rate Chemistry is available when Laminar or Zero Equation turbulence
model is used.
In multiphase simulations, when Fluid Dependent is selected, a different combustion model can
be used for each reacting fluid in the simulation. If the homogeneous multiphase model is used, all
fluids must be reacting mixtures that include reactions to allow a combustion to be modeled.
If the fluid material is defined as a reacting mixture from the material library, then the available combustion models are filtered in order to be compatible with the reactions specified in the reacting material.
If the fluid material is defined as Option is Material Definition and Composition Option is
Reacting Mixture, then the complete list of combustion models is presented and the reactions
list for the mixture has to be specified. Only those reactions from the material library will be available
that are compatible with the selected combustion model.
Depending on the selected combustion model, additional options (such as Autoignition Model,
NO Model, and Chemistry Post-Processing) and parameters may be available. For details, see
Combustion Modeling in the CFX-Solver Modeling Guide.
12.4.2.4.1. Soot Model
When a combustion model is selected, you can optionally enable the Magnussen soot model to account
for the formation of soot. In multiphase simulations, this model appears on the fluid-specific tab for
each fluid that uses a combustion model.
A Fuel and Soot Material is required, and the following optional parameters can also be set:
•
Fuel Consumption Reaction
•
Fuel Carbon Mass Fraction
•
Soot Density
•
Soot Particle Mean Diameter
For details, see Soot Model in the CFX-Solver Modeling Guide.
12.4.2.5. Thermal Radiation Model
If a heat transfer model other than None has been selected, you can model thermal radiation. If a radiation model is selected, you must make sure that the radiation properties for that fluid have been set
in the Material details view. For details, see Material Properties Tab (p. 263). Radiation is not supported
for multiphase simulations in CFX.
The four radiation models available in CFX are:
•
Rosseland
•
P1
•
Discrete Transfer
•
Monte Carlo
A Spectral Model can be selected for all radiation models. If the Multigray or Weighted Sum of
Gray Gases representation is selected for the Spectral Model, then you should create the required
number of gray gases.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
117
Chapter 12: Domains
1.
Click Add new item
to add a new gray gas. (You can click Delete
to delete a highlighted gray
gas.)
2.
Set the Weight and Absorption Coefficient for each gray gas.
For details, see Multigray/Weighted Sum of Gray Gases in the CFX-Solver Modeling Guide.
Alternatively, if the Multiband representation is selected, you should create Spectral Bands:
1.
Click Add new item
to add a new spectral band. (You can click Delete
to delete a highlighted
spectral band.)
2.
Set Option to either Frequency, Wavelength or Wavenumber.
3.
Enter upper and lower limits for the option selected.
This defines the range of the spectral band. For details, see:
•
Multiband in the CFX-Solver Modeling Guide
•
Spectral Model in the CFX-Solver Modeling Guide
•
Radiation Modeling in the CFX-Solver Modeling Guide.
12.4.2.6. Electromagnetic Model
The Electromagnetic Model enables you to define:
Electric Field Model
Option can be set to None, Electric Potential, or User Defined.
Magnetic Field Model
Option can be set to None, Magnetic Vector Potential, or User Defined.
If a user-defined model is selected, you must make sure that the electromagnetic properties have been
set in the Material details view. For details, see Material Properties Tab (p. 263). Electromagnetic models
are supported for multiphase simulations only if homogeneous.
For more information on electromagnetic theory, see Electromagnetic Hydrodynamic Theory in the CFXSolver Theory Guide.
12.4.2.7. Component Details
If your fluid contains more than one component (that is, you are using a variable composition or reacting
mixture, or HCF fuel, created in the Material details view), then Component Details will need to be
set on the Fluid Models tab. If using the Algebraic Slip Multiphase model (ASM), the settings are specified
in this view as well. For details, see Algebraic Slip Model (ASM) in the CFX-Solver Modeling Guide. When
a non-ASM multiphase model is used, the Component Details form appears on the fluid-specific tabs.
•
Select each component in turn and set the required option.
•
Select the type of equation to solve for this component as Automatic, Transport Equation,
Constraint, Algebraic Equation or Algebraic Slip. A description of the multiphase
model is available in:
– Algebraic Slip Model (ASM) in the CFX-Solver Modeling Guide
–
118
Component Domain Settings in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
•
If you have chosen to solve a transport equation for the component, you can optionally enter a value
for Kinematic Diffusivity. If you do not set Kinematic Diffusivity, then the Bulk Viscosity value is
used.
•
If you have chosen to solve a transport equation or an Algebraic Slip component, you can optionally
set a component dependent Turbulent Schmidt Number by enabling the Turbulent Flux Closure
check box. If you do not select Turbulent Flux Closure, the value from Turbulence > Turbulent Flux
Closure for Heat Transfer will be used.
The Component Details specify the model used to calculate the mass fraction of each component
throughout the domain. For details, see Component Domain Settings in the CFX-Solver Modeling Guide.
12.4.2.8. Additional Variable Details
If you have defined any Additional Variables from the Additional Variable details view, then you can
choose to include or exclude them here. An Additional Variable is included by selecting it from the
Additional Variables Details list and then enabling the check box with the name of the Additional
Variable. For details, see Additional Variables (p. 275).
If an Additional Variable is included, you must select how the Additional Variable level is calculated.
For single phase flows, the CFX-Solver can solve different variations of the conservation equations for
the variable including Transport Equation, Diffusive Transport Equation or Poisson
Equation.
For multiphase flows, the CFX-Solver can solve different variations of the conservation equations for
the variable including Homogeneous Transport Equation, Homogeneous Diffusive
Transport Equation, Homogeneous Poisson Equation or Fluid Dependent. When the
Fluid Dependent option is selected, the Additional Variable model details can be set for each fluid
on the Fluid Specific Models tab.
If a transport equation is being solved for an Additional Variable, the Turbulent Flux Closure may be
optionally specified for turbulent flow. If you do not select Turbulent Flux Closure for the Additional
Variable, the default is Option is Eddy Diffusivity and the Turb. Schmidt Num. is set to 0.9.
Alternatively, you can define the variable value algebraically using CEL by selecting the Algebraic
Equation option. Note that the Algebraic Equation option is not available for homogeneous
Additional Variables. In addition, only specific Additional Variables are permitted to be homogeneous.
For details, see Additional Variables in the CFX-Solver Modeling Guide.
12.4.3. Polydispersed Fluid Tab
The Polydispersed Fluid tab for a domain object contains settings that define the properties of polydispersed (MUSIG) fluids. It is accessible by selecting the Polydispersed Fluid option for Fluid and
Particle Definitions... > <fluid definition> > Morphology on the Basic Settings tab.
For details, see Polydispersed, Multiple Size Group (MUSIG) Model in the CFX-Solver Modeling Guide.
12.4.4. Fluid Specific Models Tab
The Fluid Specific Models tab contains settings for fluid-specific properties. It appears for multiphase
simulations and when particles are included in the domain.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
119
Chapter 12: Domains
Which options are available depends on the simulation set up, including the type and number of fluids
used in the simulation (for example, single or multicomponent, single or multiphase, reacting or nonreacting), and whether Additional Variables have been created.
12.4.4.1. Fluid List Box
This list box is used to select a fluid (which can, in some cases, represent a solid). The rest of the tab
contains settings for the selected fluid.
12.4.4.2. Kinetic Theory
The Kinetic Theory settings control the solid particle collision model. When you set Kinetic Theory to
Kinetic Theory, you should set the granular temperature model and radial distribution function.
CFX-Pre will also set the Solid Pressure Model, Solid Bulk Viscosity, and the Solid Shear Viscosity
settings to Kinetic Theory.
For details on these settings:
See:
Granular temperature model
Granular Temperature
Radial distribution function
Kinetic Theory Models for Solids Pressure
Solid pressure model
Solids Pressure
Solid bulk viscosity
Solids Bulk Viscosity
Solid shear viscosity
Solids Shear Viscosity
For modeling information about solid particle collision models, see Solid Particle Collision Models in
the CFX-Solver Modeling Guide.
For theoretical information about solid particle collision models, see Solid Particle Collision Models in
the CFX-Solver Theory Guide.
12.4.4.3. Heat Transfer
If you have set Heat Transfer to Fluid Dependent on the Fluid Models tab, the Heat Transfer
options appear on the fluid-specific tabs for each Eulerian phase. The available options are similar to
those in the single-phase case. For details, see Heat Transfer (p. 114). If the heat transfer occurs between
two fluids, then additional information must be entered on the Fluid Pairs tab.
Important
If a compressible transient flow is undertaken with only one iteration per time step, then the
solution can be incorrect if the Heat Transfer option is not set to Total Energy, or if heat
transfer is not included in the simulation. This is due to the CFX-Solver not extrapolating the
pressure at the start of the time step in these circumstances. This means that density is not
extrapolated, and so the solver cannot calculate an accurate value for the time derivative of
density on the first iteration. The workaround for this problem is to either run with at least
two iterations per time step, or to use the Total Energy option for Heat Transfer.
The Total Energy heat transfer model is not available for multiphase simulations because highspeed compressible multiphase flow is not supported. For details, see Heat Transfer in the CFX-Solver
120
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
Modeling Guide. Additional information on heat transfer between phases is available in Interphase Heat
Transfer in the CFX-Solver Modeling Guide.
12.4.4.3.1. Heat Transfer Option: Particle Temperature
When heat transfer is modeled, heat transfer for the particles is enabled by setting this option to
Particle Temperature. For details, see Heat Transfer in the CFX-Solver Modeling Guide.
12.4.4.4. Turbulence Model
If you have set Turbulence to Fluid Dependent on the Fluid Models tab, the Turbulence Model
option appears on the fluid-specific tabs for each Eulerian phase. The models available are similar to
those available in single-phase simulations, with the following exceptions:
•
For dispersed fluid, or dispersed/polydispersed solid phases, only the Dispersed Phase Zero
Equation, Laminar or Zero Equation models are available. The Dispersed Phase Zero Equation
model is the recommended choice. For details, see Phase-Dependent Turbulence Models in the CFXSolver Modeling Guide.
•
The LES and DES models are available for transient simulations for the continuous phase.
For details, see Turbulence (p. 115).
12.4.4.5. Turbulent Wall Functions
The turbulent wall functions are selected automatically, but apply only to the current fluid. For details,
see Wall Function (p. 116).
12.4.4.6. Combustion Model
If you have set the reaction or combustion model to Fluid Dependent on the Fluid Models tab, the
Reaction or Combustion Model option can appear on the Fluid Specific Models tab for each Eulerian
phase. You will only be able to pick a combustion model for fluids that are reacting mixtures. The
models available are similar to those available in single-phase simulations. For details, see:
•
Phasic Combustion in the CFX-Solver Modeling Guide
•
Reaction or Combustion Model (p. 116).
12.4.4.7. Erosion Model
The erosion properties specified on this form are applied to all wall boundaries. The wall boundaries
can also have erosion properties set to override the global settings specified here. For details, see Erosion
in the CFX-Solver Modeling Guide.
12.4.4.8. Fluid Buoyancy Model
This option is available for multiphase buoyant flows and/or buoyant flows that include particles (set
on the Basic Settings tab). For details, see Buoyancy in Multiphase Flow in the CFX-Solver Modeling
Guide.
12.4.4.9. Solid Pressure Model
This is available for Dispersed Solid Eulerian phases (phases with Dispersed Solid as the
Morphology setting). For details, see Solid Pressure Force Model in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
121
Chapter 12: Domains
12.4.4.10. Component Details
This is available for each Eulerian phase in the simulation that is a mixture of more than one component.
It does not apply to fluids or solids using the particle tracking model. The options available are the
same as those on the Fluid Models tab in a single-phase simulation. For details, see Component Details (p. 118).
If the component transfer occurs between two fluids, then additional information must be entered on
the Fluid Pairs tab. This is only possible when more than one multicomponent fluid exists in a simulation.
For details, see Interphase Species Mass Transfer in the CFX-Solver Modeling Guide.
12.4.4.11. Additional Variable Models
This is available for each Eulerian phase in the simulation when Additional Variables have been created
as well as selected and set to Fluid Dependent on the Fluid Models tab. The options available are
the same as those on the Fluid Models tab in a single-phase simulation. It does not apply to fluids or
solids using the particle tracking model. For details, see Additional Variable Details (p. 119).
If the Additional Variable transfer occurs between two fluids, then additional information must be
entered on the Fluid Pairs tab. This is possible only when more than one phase in a simulation includes
Additional Variables. For details, see Additional Variables in Multiphase Flow in the CFX-Solver Modeling
Guide.
12.4.5. Fluid Pair Models Tab
The Fluid Pairs tab appears for multiphase simulations and/or when particles are included in the domain.
It is used to specify how the fluids interact in a multiphase simulation and how particles interact with
the fluids when particles are included.
For details, see Interphase Radiation Transfer in the CFX-Solver Modeling Guide.
12.4.5.1. Fluid Pair List box
The top of the Fluid Pair Models tab shows a list of all the phase pairs in the simulation. A phase pair
will exist when the morphology of the pair is Continuous Fluid | Continuous Fluid, Continuous Fluid
| Dispersed Fluid or Continuous Fluid | Dispersed Solid. If particles have also been included, then a
pair will exist for each Continuous Fluid | Particle pair. You should select each pair in turn and set the
appropriate options.
The options available will vary considerably depending on your simulation. Many options are not
available when the homogeneous multiphase model is used. This is because the interphase transfer
rates are assumed to be very large for the homogeneous model and do not require further correlations
to model them.
12.4.5.2. Particle Coupling
This only applies to Continuous Fluid | Particle pairs. For details, see Particle Fluid Pair Coupling Options
in the CFX-Solver Modeling Guide.
12.4.5.3. Surface Tension Coefficient
You can optionally provide a Surface Tension Coefficient. This should be set in either of the following
two cases:
122
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
•
For a Continuous Fluid | Dispersed Fluid pair when you want to model the Drag Force using either
the Grace or Ishii Zuber models. The flow must also be Buoyant to allow these models to be selected. For details, see Interphase Drag for the Particle Model in the CFX-Solver Modeling Guide.
•
When you want to use the surface tension model. This model is only available when Standard has
been selected as the Free Surface Model on the Fluid Models tab.
You can set a Surface Tension Coefficient in other cases, but it will not be used in your simulation. It
does not apply to Continuous Fluid | Particle pairs.
For details, see Surface Tension in the CFX-Solver Modeling Guide.
12.4.5.4. Surface Tension Force Model
You can model the surface tension force that exists at a free surface interface. This model applies to all
morphology combinations for Eulerian | Eulerian pairs. You must also specify a Surface Tension Coefficient and select the Primary Fluid. For liquid-gas free surface flows, the primary fluid should be the
liquid phase.
For details, see Surface Tension in the CFX-Solver Modeling Guide.
12.4.5.5. Interphase Transfer Model
This can be selected as one of the following:
12.4.5.5.1. Particle Model
This model assumes a continuous phase fluid containing particles of a dispersed phase fluid or solid. It
is available when the morphology of the pair is Continuous Fluid | Dispersed Fluid or Continuous
Fluid | Dispersed Solid. For details, see The Particle Model in the CFX-Solver Modeling Guide.
12.4.5.5.2. Mixture Model
This model is only available when the morphology of the pair is Continuous Fluid | Continuous Fluid.
An Interface Length Scale is required. It is usually used as a first approximation or combined with a
custom interface transfer model. For details, see The Mixture Model in the CFX-Solver Modeling Guide.
12.4.5.5.3. Free Surface Model
This model is available when the free surface model is selected. For details, see The Free Surface Model
in the CFX-Solver Modeling Guide. For free surface flow, the particle model is also available if the phase
pair is Continuous Fluid | Dispersed Fluid, and the mixture model is also available if the phase pair
is Continuous Fluid | Continuous Fluid.
12.4.5.5.4. None
For homogeneous multiphase flow in which there is no interphase transfer of any type, the interphase
transfer model is not relevant and None may be selected.
12.4.5.6. Momentum Transfer
There are a variety of momentum transfer that can be modeled, including the drag force and non-drag
forces, which include lift force, virtual mass force, wall lubrication force and turbulent dispersion force.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
123
Chapter 12: Domains
12.4.5.6.1. Drag Force
This option applies to all morphology pair combinations including Continuous Fluid | Particle pairs,
but does not apply when the Homogeneous multiphase model is active.
There are many drag force models available in CFX, but most are only applicable to certain morphology
combinations. For Continuous Fluid | Particle pairs, the available options are:
•
The Schiller-Naumann drag model.
For details, see Interphase Drag in the CFX-Solver Modeling Guide.
•
The Drag Coefficient.
For details, see Drag Force for Particles in the CFX-Solver Modeling Guide.
•
The Ishii Zuber drag model.
For details, see Sparsely Distributed Fluid Particles: Ishii-Zuber Drag Model in the CFX-Solver Modeling
Guide and Densely Distributed Fluid Particles: Ishii-Zuber Drag Model in the CFX-Solver Modeling
Guide.
•
The Grace drag model.
For details see, Sparsely Distributed Fluid Particles: Grace Drag Model in the CFX-Solver Modeling
Guide and Densely Distributed Fluid Particles: Grace Drag Model in the CFX-Solver Modeling Guide.
12.4.5.6.2. Particle User Source
The Particle User Source check box is available when any User Routines of type Particle User Routines
exist. For details, see:
•
Particle User Routines (p. 295)
•
Particle User Sources in the CFX-Solver Modeling Guide.
12.4.5.6.3. Lift Force
The lift force is only applicable to the Particle Model, which is active for Continuous Fluid | Dispersed (Fluid, Solid) and Continuous Fluid | Polydispersed Fluid. For details, see Lift Force in the
CFX-Solver Modeling Guide.
12.4.5.6.4. Virtual Mass Force
This option applies to Continuous Fluid | Dispersed Fluid pairs using the Particle Model, and to
Continuous Fluid | Particle pairs, but does not apply when the Homogeneous multiphase model is
active. For details, see Virtual Mass Force in the CFX-Solver Modeling Guide.
12.4.5.6.5. Wall Lubrication Force
This option is only applicable to the Particle Model. For details, see Wall Lubrication Force in the
CFX-Solver Modeling Guide.
12.4.5.6.6. Turbulent Dispersion Force
This applies to Continuous Fluid | Dispersed Fluid, Continuous Fluid | Polydispersed Fluid and
Continuous Fluid | Dispersed Solid pair combinations for Eulerian | Eulerian pairs, but does not apply
124
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
when the Homogeneous multiphase model is active. In these cases, the Lopez de Bertodano model is
used. For details, see Interphase Turbulent Dispersion Force in the CFX-Solver Modeling Guide.
When particle tracking is used, the turbulent dispersion force also applies to Continuous Fluid | Particle
pairs. In these cases, the Particle Dispersion models is used. For details, see Turbulent Dispersion Force
in the CFX-Solver Modeling Guide.
12.4.5.6.7. Pressure Gradient Force
This option is only available for Particle Tracking simulations. For details, see Pressure Gradient Force
in the CFX-Solver Modeling Guide.
12.4.5.7. Turbulence Transfer
This model is available for Continuous Fluid | Dispersed Fluid, Continuous Fluid | Polydispersed
Fluid and Continuous Fluid | Dispersed Solid pair combinations for Eulerian | Eulerian pairs, but
does not apply when the Homogeneous multiphase model is active and is not available for Continuous
Fluid | Particle pairs. For details, see Turbulence Enhancement in the CFX-Solver Modeling Guide.
12.4.5.8. Heat Transfer
This applies to all morphology combinations for Eulerian | Eulerian and Continuous Fluid | Particle
pairs, but does not apply when the Homogeneous multiphase model is active.
For details, see Interphase Heat Transfer in the CFX-Solver Modeling Guide for multiphase applications
and Interphase Heat Transfer in the CFX-Solver Modeling Guide for particle transport modeling.
12.4.5.9. Mass Transfer
Mass transfer can occur in homogeneous and inhomogeneous Eulerian multiphase flows. For such flows,
you can set the Mass Transfer option to one of the following:
•
None
•
Specified Mass Transfer
This is an advanced option that allows you to define your own mass transfer sources. For details,
see User Specified Mass Transfer in the CFX-Solver Modeling Guide.
•
Phase Change
This models mass transfer due to phase change, such as boiling, condensation, melting or solidification. For details, see Thermal Phase Change Model in the CFX-Solver Modeling Guide.
•
Cavitation
Vapor formation in low pressure regions of a liquid flow (cavitation) can be modeled using the
Rayleigh Plesset model or, for advanced users, a user-defined model. For details, see Cavitation
Model in the CFX-Solver Modeling Guide.
12.4.5.10. Additional Variable Pairs
Additional Variable Pairs details describe the way in which Additional Variables interact between
phases. It applies to all morphology combinations for Eulerian | Eulerian pairs, but does not apply
when the Homogeneous multiphase model is active.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
125
Chapter 12: Domains
Only Additional Variable pairs where both are solved using the Transport Equation and have a Kinematic Diffusivity value set can be transferred between phases. These options are set on the fluidspecific tabs for each phase.
For example, consider two phases, Phase A and Phase B, and two Additional Variables, AV1 and
AV2.
•
AV1 uses a Transport Equation with diffusion in Phase A and is unused in Phase B.
•
AV2 uses an Algebraic Equation in Phase A and uses a Transport Equation with diffusion in Phase B.
Additional Variable interphase transfer can only occur between Phase A / AV1 and Phase B / AV2.
For details, see Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide.
12.4.5.11. Component Pairs
12.4.5.11.1. Eulerian | Eulerian Pairs
You can model transfer of components between phases for Eulerian | Eulerian pairs, when both fluids
are multicomponent mixtures of any type (except fixed composition mixtures). Mixtures are created in
the Material details view. For example, to create a Variable Composition Mixture, see Material Details View: Variable Composition Mixture (p. 267). Component (or species) transfer enables you to
model processes such as evaporation, absorption and dissolution.
To specify the component transfer model, you should select the component pair from the list on the
Fluid Pairs tab and then select the associated toggle. The first component of the component pair corresponds to the first fluid in the fluid pairs list.
Option can be set to Two Resistance or Ranz Marshall. For details, see:
•
Two Resistance Model in the CFX-Solver Modeling Guide
•
Ranz Marshall in the CFX-Solver Modeling Guide.
The choice of interfacial equilibrium model depends on the process that you are modeling. For details,
see Interfacial Equilibrium Models in the CFX-Solver Modeling Guide.
The Fluid1 and Fluid2 Species Mass Transfer options are used to choose a correlation to
model the mass transfer coefficient on each side on the interface. For details, see Species Mass Transfer
Coefficients in the CFX-Solver Modeling Guide.
12.4.5.11.2. Continuous | Particle Pairs
Selecting the toggle enables mass transfer between the two phases.
The options for mass transfer are:
•
Ranz Marshall. For details, see Ranz Marshall in the CFX-Solver Modeling Guide.
•
Liquid Evaporation Model. For details, see Liquid Evaporation Model in the CFX-Solver Modeling
Guide. For oil evaporation, the Light Oil check box should be selected. For details, see Liquid Evaporation
Model: Oil Evaporation/Combustion in the CFX-Solver Modeling Guide.
•
None
For details on these options, see:
126
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
•
Latent Heat in the CFX-Solver Modeling Guide
•
Particle User Source in the CFX-Solver Modeling Guide.
The drop-down list will contain any User Particle Routines you have created. For details, see Particle
User Routines (p. 295).
Mass transfer between a species in a particle phase and a species in the continuous phase is possible.
For example, consider liquid water from a particle evaporating into gaseous H20 in a continuous phase
mixture. The particle can be a pure substance or variable composition mixture.
12.4.5.12. Particle Breakup
The Particle Breakup models allow you to simulate the breakup of droplets due to external aerodynamic
forces. The droplet breakup models are set on a per fluid-pair basis. By default, the Use Liu Dynamic
Drag Modification option is activated for the TAB, ETAB and CAB breakup models, whereas the Use
Schmehl Dynamic Drag Law option is activated for the Schmehl breakup model. See Particle Breakup
Model in the CFX-Solver Modeling Guide for details on the available particle breakup models.
12.4.5.13. Particle Collision
The particle collision model enables you to simulate dense gas-solid flows with high mass-loading while
the particle volume fraction is still low. Select either Sommerfeld Collision Model or User
Defined and specify values for the particle collision parameters outlined below:
Sommerfeld Collision Model
•
Coefficient of Restitution: Enter a numerical quantity or CEL based expression to specify
the value of coefficient of restitution for inter-particle collisions. A value of ‘1.0’ means a fully elastic
collision, while a value of ‘0.0’ would result in an inelastic collision.
•
Static Friction Coefficient and Kinetic Friction Coefficient: Enter a numerical quantity or CEL based expression to specify values of coefficients of friction for inter-particle
collisions.
See Implementation Theory in the CFX-Solver Theory Guide for more information on setting up
Coefficient of Restitution, Static Friction Coefficient, and Kinetic
Friction Coefficient.
User Defined
This option is available only if you have created a particle user routine to set up the model. Specify the
name of Particle User Routine and select input arguments and type of particle variables returned to
the user routine from the Arguments and Variable List drop-down list, respectively. See Particle User
Routines in the CFX-Pre User's Guide for information on setting up a particle user routine.
For additional information, see Particle Collision Model in the CFX-Solver Modeling Guide and the following
topics available under Particle Collision Model in the CFX-Solver Theory Guide:
•
Introduction to the Particle Collision Model
•
Implementation of a Stochastic Particle-Particle Collision Model in ANSYS CFX (includes the discussion
on the implementation theory, particle variables, and virtual collision partner)
•
Particle Collision Coefficients Used for Particle-Particle Collision Model
•
Range of Applicability of Particle-Particle Collision Model
•
Limitations of Particle-Particle Collision Model in ANSYS CFX
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
127
Chapter 12: Domains
12.4.6. Solid Models Tab
The Solid Models tab sets the models that apply to solid domains and to the solid material in a porous
domain. The models chosen can vary between each domain, but if radiation is modeled, then all fluid
domains must also model radiation. For details, see Using Multiple Domains (p. 106).
12.4.6.1. Heat Transfer
The Thermal Energy model and Isothermal model are available for the solid domain. If you do
not want to model heat transfer for the domain, then set Heat Transfer > Option to None.
For details, see Conjugate Heat Transfer in the CFX-Solver Modeling Guide.
12.4.6.2. Thermal Radiation Model
You can use only the Monte Carlo option to model radiation in a solid domain. The options available
are the same as for the Monte Carlo model in a fluid domain. For details, see Thermal Radiation
Model (p. 117).
You cannot model radiation in a porous domain.
12.4.6.3. Electromagnetic Model
The Electromagnetic Model enables you to define:
Electric Field Model
Option can be set to None, Electric Potential, or User Defined.
For a User Defined setting, you have to specify the electric field strength for the X, Y, and Z
directions.
Magnetic Field Model
Option can be set to None, Magnetic Vector Potential, or User Defined.
For the Magnetic Vector Potential option, you can specify External Magnetic Field settings
using Cartesian or cylindrical components. Using the User Defined option will enable you to
specify the induced magnetic field model in the X, Y, and Z directions.
If a user-defined model is selected, you must make sure that the electromagnetic properties have been
set in the Material details view. For details, see Material Properties Tab (p. 263). Electromagnetic models
are supported for multiphase simulations only if homogeneous.
For more information on electromagnetic theory, see Electromagnetic Hydrodynamic Theory in the CFXSolver Theory Guide.
12.4.6.4. Additional Variables Models
See Additional Variables.
12.4.6.5. Solid Motion
You can model the motion of a solid that moves relative to its reference frame by selecting the Solid
Motion option and specifying a velocity.
128
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
Examples of such motions include:
•
A continuous sheet of material moving along a conveyor belt
•
A material being continuously extruded
•
An axisymmetric solid that rotates about its symmetry axis
You can specify the velocity using one of the following methods:
•
Cartesian velocity components
You must specify values for U, V, and W.
•
Cylindrical velocity components
You must specify values for Axial Component, Radial Component, and Theta Component. You
must also specify an Axis Definition.
•
Rotating
Specify an Angular Velocity and an Axis Definition.
The velocity that you specify is interpreted as being relative to the domain motion which is, in turn,
relative to the coordinate frame; both of these are specified on the Basic Settings tab for the domain.
The solid motion model does not involve changing the mesh. Instead, motion of the solid is simulated
by imposing a velocity field in the solid domain. The velocity field causes the advection of energy and
Additional Variables as applicable.
On interfaces to other domains (fluid-solid or solid-solid interfaces) the solid must move only tangentially
to its surface. On an external boundary, if the solid has a velocity component normal to the surface,
then consider activating the advection term(s) on the boundary condition for that surface, by visiting
the Boundary Details tab and selecting Solid Motion > Boundary Advection. For details on setting
up boundary advection on a wall, see Solid Motion: Wall (p. 155).
Note
•
Most solid motion cases will involve setting either non-stationary domain motion (on the
Basic Settings tab) or activating the Solid Motion setting (on the Solid Models tab) but
not both.
•
If you have a solid with Solid Motion activated that meets a fluid domain at a fluid-solid
interface, then you must explicitly set the wall boundary condition applied to the fluid side
of the interface to have a wall velocity corresponding to the solid motion, as required.
12.4.7. Porosity Settings Tab
The Porosity Settings tab is where the general description of a porous domain is specified for the
simulation.
12.4.7.1. Area Porosity
Area Porosity represents the fraction of physical area that is available for the flow to go through. The
default setting is Isotropic.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
129
Chapter 12: Domains
12.4.7.2. Volume Porosity
Volume Porosity is the local ratio of the volume of fluid to the total physical volume.
12.4.7.3. Loss Models
The porous loss options are:
•
Isotropic Loss
For the isotropic loss model, the loss may be specified using either one of the following methods:
•
–
Permeability And Loss Coefficient
–
Linear And Quadratic Resistance Coefficients
Directional Loss
Specify the streamwise direction via Cartesian or cylindrical components (in the coordinate frame
specified on the Basic Settings tab).
The loss in the streamwise direction can be specified using one of the following options:
–
Permeability And Loss Coefficient
–
Linear And Quadratic Resistance Coefficients
–
No Loss
The loss in the transverse directions can be specified using one of the following options:
•
–
Streamwise Coefficient Multiplier
–
Permeability and Loss Coefficient
–
Linear and Quadratic Resistance Coefficients
–
No Loss
None
When specifying the loss coefficients, it is important to set the Loss Velocity Type properly. For details,
see Porous Momentum Loss Models in the CFX-Solver Theory Guide.
12.4.7.4. Contact Area Model
This setting is available only when the porous domain has a solid phase.
When there is more than one fluid in a porous domain that has a solid phase, specify the contact area
model to indicate how the contact area between a given fluid and the solid is to be calculated.
The options are:
•
Use Volume Fraction
This option makes use of the volume fraction of each fluid to calculate the contact area between
that fluid and the solid.
•
Fluid Dependent
This option enables the direct specification of the contact area fraction for each fluid. The area
fractions must sum to unity.
130
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
12.4.7.5. Fluid Solid Area Density
This setting is available only when the porous domain has a solid phase.
Specify the fluid-solid area density, which is the contact area per unit volume, where the contact area
is the surface area of the solid in contact with the fluid(s).
12.4.7.6. Fluid Solid Heat Transfer
This setting is available only when the porous domain has a solid phase.
Specify the overall heat transfer coefficient for heat transfer between the fluid(s) and the solid. This is
analogous to the heat transfer coefficient between fluids in an inhomogeneous multiphase case, as
described in Inhomogeneous Interphase Heat Transfer Models.
12.4.7.7. Additional Variable Pair Details
This setting is available only when the porous domain has a solid phase.
Specify pairs of the same Additional Variable to enable the Additional Variable transfer between the
solid and the fluid(s).
The options are:
•
Additional Variable Transfer Coefficient
This option applies a bulk value of the Additional Variable transfer coefficient between the fluid(s)
and the solid.
•
Fluid Dependent
This option enables the direct specification of the Additional Variable transfer coefficient for each
fluid.
The Additional Variable transfer coefficient is analogous to the transfer coefficient between fluids in an
inhomogeneous multiphase case. For details, see Additional Variable Interphase Transfer Models in the
CFX-Solver Modeling Guide and Additional Variables in Multiphase Flow in the CFX-Solver Theory Guide.
12.4.8. Particle Injection Regions Tab
Injection regions are used to define locators anywhere within a domain, and can be set up as spheres,
cones, or using a custom Fortran subroutine. For details, see Particle Injection Regions in the CFX-Solver
Modeling Guide.
12.4.8.1. Particle Injection Regions List Box
This list box is used to select Particle Injection Regions for editing or deletion. Particle Injection Regions
can be created or deleted with the icons that appear beside the list box.
12.4.8.2. Coordinate Frame
In some cases it may be useful to specify injection quantities using coordinates from a coordinate frame
other than the global default frame (Coord 0). To do this, choose a local coordinate frame from the
drop-down list. You can then set the injection center and the injection direction relative to the selected
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
131
Chapter 12: Domains
coordinate frame. In a typical application, it makes sense to use a coordinate frame that has a principal
axis aligned with the general spray direction.
Note
The coordinate frame of a particle injection region is independent of the coordinate frame
of the domain.
Note
In the case of user defined injection, the particle position and the injection velocity – if returned from the user routine – refer to the global coordinate frame Coord 0 rather than
to the one specified under Coordinate Frame.
12.4.8.3. Fluid: List Box
This list box is used to select a particle material in order to apply it to the injection region and define
its properties for the injection region.
12.4.8.4. [fluid name] Check Box
This check box determines whether or not the particle is to be injected over the selected injection region.
For multicomponent particles, specify the mass fraction of each. Other quantities are optional and are
the same as found on the Fluid Values tab. For details, see Fluid Values for Inlets and Openings (p. 158).
12.4.8.4.1. Injection Method
The following table outlines various settings available on Particle Injection Regions tab. The settings
are marked as required or optional based on the type of injection method chosen.
Injection Method
Settings for Injection Method
Cone
Injection Center
Required
Injection Velocity Magnitude
Radius of Injection Sphere
Number of Positions
Cone with
Primary Breakup
Sphere
Required
Required
a
Required
Optional
a
a
Required
Particle Diameter Distribution
Optional
Particle Mass Flow Rate
Optional
Required
Optional
Required
Cone Definition
For details, see Settings for Cone Definition (p. 133).
Required
Injection Direction
Injection Velocity
132
Required
Required
Required
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Optional
User Interface
Injection Method
Cone
Settings for Injection Method
Cone with
Primary Breakup
Sphere
For details, see Settings for Injection Velocity (p. 133).
Particle Primary Breakup
Required
For details, see Settings for Particle Primary
Breakup (p. 134).
Nozzle Definition
b
Required
a
Enter a numerical quantity or CEL expression for the indicated parameter.
Nozzle Definition: Select either Ring Nozzle or Full Nozzle and specify the values to define the nozzle.
b
For details, see the following topics in the CFX-Solver Modeling Guide:
•
Particle Injection Regions (includes description of various types of cone locators)
•
Number of Positions
•
Particle Diameter Distribution
•
Particle Mass Flow Rate
12.4.8.4.1.1. Settings for Cone Definition
Settings
Cone Angle
Point
Cone
a
Dispersion Angle
Hollow
Cone
Ring
Cone
Full
Cone
Required
a
Optional
Radius of Injection Plane
a
Optional
Required
Required
Inner Radius Of Plane
a
Required
Outer Radius Of Plane
a
Required
a
Enter a numerical quantity or CEL expression for the indicated parameter.
For details, see Cone in the CFX-Solver Modeling Guide.
12.4.8.4.1.2. Settings for Injection Velocity
The Injection Velocity options are:
•
Velocity Magnitude
Specify the component of velocity normal to the 2D injection region. Note that the normal direction
is specified by the Injection Direction settings.
Specify the cone angle, measured as the angle between the axis of the cone (which, for the Velocity Magnitude option, is normal to the 2D injection region) and one side of the cone.
•
Cartesian Components
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
133
Chapter 12: Domains
Specify the particle velocity components in Cartesian coordinates. These coordinates are in the
coordinate frame specified for the particle injection region. The velocity components can be expressions.
•
Cylindrical Components
Specify the particle velocity components in cylindrical coordinates. These coordinates are in the
coordinate frame specified for the particle injection region. The velocity components can be expressions.
You can put swirl into the flow of injected particles by specifying a non-zero theta (circumferential)
component of velocity.
•
Zero Slip Velocity
Particles are injected at the local velocity of the continuous phase.
12.4.8.4.1.3. Settings for Particle Primary Breakup
Settings
Cone Angle
a b
Coefficient of Contraction
a
Injection Total Pressure
a
Blob
Method
Enhanced
Blob Method
Lisa
Model
Required
Required
Required
Required
Required
Injection Pressure Difference
a
Pressure Probe Normal
Distance
a
Required
Required
Required
Required
Required
Density Probe Normal
Distance
Length/Diameter Ratio
Particle Material Vapor
Pressure
Turbulence Induced Atomization
Required
Required
Critical Weber Number
Optional
Short Wave Ligament
Factor
Optional
Long Wave Ligament
Factor
Optional
Droplet Diameter Size
Factor
Optional
Swirl Definition
Optional
Form Loss Coefficient
Optional
C1 Constant
Optional
C2 Constant
Optional
134
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
Settings
Blob
Method
Enhanced
Blob Method
Lisa
Model
Turbulence Induced Atomization
C3 Constant
Optional
C4 Constant
Optional
CA1 Constant
Optional
K1 Constant
Optional
Average Turbulent Energy Dissipation Factor
Optional
Turbulent Length Scale
Power Factor
Optional
Nozzle Discharge Coefficient
Required
a
Enter a numerical quantity or CEL expression for the indicated parameter.
Cone Angle: Specify a fixed cone angle or select Reitz and Bracco option to set a correlation to compute the injection angle based
on the nozzle geometry.
b
For details, see Cone with Primary Breakup in the CFX-Solver Modeling Guide.
12.4.9. Initialization Tab
Initialization can be set on a domain or global basis; the available options are the same. For details, see
Initialization (p. 167).
The Initialization tab for the domain sets domain initial conditions. These will override any settings
made in the Global Initialization details view. Any domain for which initialization is not set will use
the global initial conditions.
12.4.10. Solver Control Tab
For immersed solid domains, the Solver Control tab contains the Immersed Solid Control settings. For
details, see Immersed Solid Control (p. 202).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
135
136
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 13: Domain Interfaces
Domain interfaces have multiple purposes:
•
Connecting domains or assemblies
Domain interfaces are required to connect multiple unmatched meshes within a domain (for example,
when there is a hexahedral mesh volume and a tetrahedral mesh volume within a single domain)
and to connect separate domains.
•
Modeling changes in reference frame between domains
This occurs when you have a stationary and a rotating domain or domains rotating at different
rates.
•
Creating periodic interfaces between regions
This occurs when you are reducing the size of the computational domain by assuming periodicity
in the simulation.
•
Creating thin surfaces
Thin surfaces enable you to model physics such as heat transfer across a thin material or gap
without needing to explicitly mesh the surface. For example, thin surfaces can be used to model
contact resistance at a solid-solid interface, a thin film on a fluid-solid interface, or a thin baffle at
a fluid-fluid interface.
Interface boundaries are created automatically for each domain interface. For details, see Interface
Boundary Conditions (p. 163).
Additional information about domain interfaces is provided in Overview of Domain Interfaces in the
CFX-Solver Modeling Guide.
Note
If you are running a simulation with ANSYS Multi-field coupling to the ANSYS solver, you will
need to create fluid-solid interfaces with the fluid side in CFX and the solid side in ANSYS.
Such an interface is actually an external boundary so far as CFX-Solver is concerned, as it lies
on the boundary of the CFX domain(s). You should create a Boundary Condition, not a Domain
Interface, when setting up such an interface.
13.1. Creating and Editing a Domain Interface
To create a domain interface:
1.
Select Insert > Domain Interface from the main menu or by clicking Domain Interface
on the
main toolbar.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
137
Chapter 13: Domain Interfaces
2.
Enter a new name, if required, using the rules described in Valid Syntax for Named Objects (p. 55) and
click Apply.
To edit an existing domain interface:
1.
Right-click the domain interface's name in the Outline view.
2.
Select Edit. The details view for the domain interface appears.
For more information on the edit command, see Outline Tree View (p. 5).
The details view describes the characteristics of a domain interface on a series of tabs:
•
Domain Interface: Basic Settings Tab (p. 138)
•
Domain Interface: Additional Interface Models Tab (p. 140).
13.1.1. Domain Interface: Basic Settings Tab
The Basic Settings tab is where you define the domain interface. It is accessible by clicking Domain Interface
, or by selecting Insert > Domain Interface.
13.1.1.1. Interface Type
•
Fluid Fluid
Connects two fluid domains or makes a periodic connection between two regions in a fluid domain.
•
Fluid Porous
Connects a fluid domain to a porous domain.
•
Fluid Solid
Connects a fluid domain to a solid domain.
•
Porous Porous
Connects two porous domains or makes a periodic connection between two regions in a porous
domain.
•
Solid Porous
Connects a solid domain to a porous domain.
•
Solid Solid
Connects two solid domains or makes a periodic connection between two regions in a solid domain.
The interface type you select controls the domains that are available for Interface Side 1/2.
13.1.1.2. Interface Side 1/2
13.1.1.2.1. Domain (Filter)
The domain filter is used to filter out 2D regions that are of no interest. The drop-down list contains
commonly used regions (all composite names and primitive names that are not referenced by any
138
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Domain Interface
composites) and the extended list (displayed by clicking the Ellipsis
domain.
icon) contains all regions in a
13.1.1.2.2. Region List
Region List 1 and Region List 2 allow selection of regions that form each side of the interface.
13.1.1.3. Interface Models
The interface model options (Translational Periodicity, Rotational Periodicity, and General Connection)
each require that you specify a mesh connection method as well as specialized settings for some
model options.
13.1.1.3.1. Interface Model Option: Translational Periodicity
In the case of Translational Periodicity, the two sides of the interface must be parallel to each other
such that a single translation transformation can be used to map Region List 1 to Region List 2. The
Translational Periodicity model requires no specialized settings.
For details on the Translational Periodicity model, see Translational Periodicity in the CFX-Solver Modeling
Guide.
13.1.1.3.2. Interface Model Option: Rotational Periodicity
In the case of Rotational Periodicity, the two sides of the periodic interface can be mapped by a single
rotational transformation about an axis. This is the most common case of periodicity and is used, for
example, in the analysis of a single blade passage in a rotating machine.
If a domain interface involves rotational periodicity, the axis for the rotational transformation must also
be specified in the Axis Definition area.
13.1.1.3.3. Interface Model Option: General Connection
In the case of a General Connection, more options apply. The settings are described below; for information about the General Connection model, see General Connection in the CFX-Solver Modeling Guide.
13.1.1.3.3.1. Frame Change/Mixing Model
13.1.1.3.3.1.1. Option
•
None
•
Frozen Rotor
•
Stage
•
Transient Rotor-Stator
For details, see Frame Change/Mixing Model in the CFX-Solver Modeling Guide.
13.1.1.3.3.1.2. Frozen Rotor: Rotational Offset Check Box
This check box determines whether or not to apply a rotational offset for one side of the interface. For
details, see Rotational Offset in the CFX-Solver Modeling Guide.
When set, enter a Rotational Offset for one side of the interface.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
139
Chapter 13: Domain Interfaces
13.1.1.3.3.1.3. Stage: Pressure Profile Decay Check Box
This option affects solution stability. For details, see Pressure Profile Decay in the CFX-Solver Modeling
Guide.
When set, enter a Pressure Profile Decay numerical quantity or CEL expression that specifies the rate
of decay of the pressure profile.
13.1.1.3.3.1.4. Stage: Constant Total Pressure Check Box
For details, see Downstream Velocity Constraint in the CFX-Solver Modeling Guide.
13.1.1.3.3.2. Pitch Change Options
The Pitch Change options are:
•
None
A pitch change option of None cannot be used for a stage interface.
•
Automatic
(applies only when Interface Models: Frame Change/Mixing Model: Option is not set to None)
•
Value
(applies only when Interface Models: Frame Change/Mixing Model: Option is not set to None)
•
Specified Pitch Angles
(applies only when Interface Models: Frame Change/Mixing Model: Option is not set to None)
For details, see Pitch Change in the CFX-Solver Modeling Guide.
13.1.1.3.3.2.1. Pitch Change: Value: Pitch Ratio
Enter the pitch ratio. For details, see Value in the CFX-Solver Modeling Guide.
13.1.1.3.3.2.2. Pitch Change: Specified Pitch Angles: Pitch Angle Side 1/2
Enter pitch angle for each side of the interface. For details, see Specified Pitch Angles in the CFX-Solver
Modeling Guide.
13.1.2. Domain Interface: Additional Interface Models Tab
The Additional Interface Models tab is where you set the Mass And Momentum, Heat Transfer,
Electric Field and Additional Variable options.
13.1.2.1. Mass And Momentum
Determines whether or not mass and momentum models are applied between the sides of the interface.
For details, see Mass and Momentum Models in the CFX-Solver Modeling Guide.
The mass and momentum options are:
•
140
Conservative Interface Flux
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Domain Interface
The Conservative Interface Flux Mass And Momentum option enables you to define the physics
across a thin surface.
•
No Slip Wall
•
Free Slip Wall
•
Side Dependent
13.1.2.1.1. Conservative Interface Flux: Interface Models
13.1.2.1.1.1. None
No models are provided for any additional mass or momentum between side 1 and side 2 of the interface.
13.1.2.1.1.2. Mass Flow Rate
Enter a numerical quantity or CEL expression that specifies the value of the mass flow rate from side 1
to side 2 of the interface.
Note
The Pressure Update Multiplier provides user control to tune convergence behavior. For details,
see Pressure Update Multiplier (p. 141).
13.1.2.1.1.2.1. Pressure Update Multiplier
Enter a numerical quantity or CEL expression that specifies the pressure update multiplier.
When imposing a mass flow rate at a domain interface, the CFX-Solver updates the pressure change to
drive the mass flow rate toward the specified value. The update is based on an internally-estimated
coefficient, which may not be optimal.
The Pressure Update Multiplier provides user control to tune convergence behavior. The default value
is 0.25. If convergence is slow (as may occur for low Reynolds number flows), consider increasing the
value. If convergence is unstable, consider decreasing the value. Note that values above 1 are permissible.
13.1.2.1.1.3. Pressure Change
Enter a numerical quantity or CEL expression that specifies the pressure change across the interface
(from side 1 to side 2). If there is a pressure drop, the specified value should be negative.
13.1.2.1.2. No Slip Wall
For a description of the options that influence flow on a wall boundary, see Mass and Momentum in
the CFX-Solver Modeling Guide.
13.1.2.1.2.1. No Slip Wall: Wall Velocity
When set, this option enables you to specify the following:
•
Wall Velocity Option: Cartesian Components (Wall U, Wall V, Wall W)
•
Wall Velocity Option: Cylindrical Components (Axial Component, Radial Component, Theta
Component), Axis Definition: Option: Coordinate Axis and Rotational Axis
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
141
Chapter 13: Domain Interfaces
•
Wall Velocity Option: Rotating Wall (Angular Velocity), Axis Definition: Option: Coordinate Axis
and Rotational Axis
13.1.2.1.3. Free Slip Wall
Free Slip Wall has no suboptions.
13.1.2.1.4. Side Dependent
Side Dependent has no suboptions.
13.1.2.2. Heat Transfer
Determines whether or not heat transfer models are applied between the sides of the interface.
The options are:
•
Conservative Interface Flux
This option enables you to define the Thermal Contact Resistance or Thin Material, which are
two ways of defining the same characteristics. That is, if you do not know the contact resistance,
you can define the thin material and its thickness and have the solver derive the resistance.
•
Side Dependent
13.1.2.2.1. Conservative Interface Flux: Interface Model
13.1.2.2.1.1. None
No models are provided for any additional heat transfer between side 1 and side 2 of the interface.
13.1.2.2.1.2. Interface Model Option: Thermal Contact Resistance
Enter a numerical quantity or CEL expression that specifies the value of the thermal contact resistance
from side 1 to side 2 of the interface.
13.1.2.2.1.3. Interface Model Option: Thin Material
Select a material and enter a numerical quantity or CEL expression that specifies the value of the
thickness of the material spanning from side 1 to side 2 of the interface.
13.1.2.2.2. Side Dependent
Side Dependent has no suboptions.
13.1.2.3. Electric Field
Determines whether or not electric field models are applied between the sides of the interface.
The options are:
•
Conservative Interface Flux
•
Side Dependent
142
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Domain Interface
13.1.2.3.1. Conservative Interface Flux: Interface Model
13.1.2.3.1.1. None
No models are provided for the electric field between side 1 and side 2 of the interface.
13.1.2.3.1.2. Interface Model Option: Electric Field Contact Resistance
Enter a numerical quantity or CEL expression that specifies the value of the electric field contact resistance
from side 1 to side 2 of the interface.
13.1.2.3.2. Side Dependent
Side Dependent has no suboptions.
13.1.2.4. Additional Variable
Determines whether or not additional variable models are applied between the sides of the interface.
The options are:
•
Conservative Interface Flux
•
Side Dependent
13.1.2.4.1. Conservative Interface Flux: Interface Model
13.1.2.4.1.1. None
No models are provided for the additional variable between side 1 and side 2 of the interface.
13.1.2.4.1.2. Interface Model Option: Additional Variable Contact Resistance
Enter a numerical quantity or CEL expression that specifies the value of the additional variable contact
resistance from side 1 to side 2 of the interface.
13.1.2.4.2. Side Dependent
Side Dependent has no suboptions.
13.1.2.5. Conditional Connection Control
Conditional Connection Control is an optional group of settings, activated by a check box. These
settings enable you to use an expression to control whether an interface is open (connected) or closed
(not connected; a wall boundary is applied).
When the Conditional Connection Control check box is active, you can select from one of these options:
•
Specified Open State
Provide a CEL expression. The connection is open when the expression evaluates to true,
and closed when the expression evaluates to false.
•
Irreversible State Change
Provide a CEL expression and an initial state. The latter is “Open” or “Closed”.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
143
Chapter 13: Domain Interfaces
The state switches once the expression evaluates to true but then remains in that opposite
state (that is, opposite to the initial condition) regardless of what happens to the expression
after that point.
For details on conditional connection control, see Conditional Connections in the CFX-Solver Modeling
Guide.
13.1.3. Domain Interface: Solid Interface Models Tab
The Solid Interface Models tab is where you set the Heat Transfer and Additional Variable boundary
conditions at the domain interface for a solid in a porous domain.
13.1.3.1. Heat Transfer
Determines whether or not heat transfer models are applied to the solid in a porous domain.
The options are:
•
Conservative Interface Flux
This option is only available if there are solids on both sides of the domain interface. It enables
you to define the Thermal Contact Resistance or Thin Material, which are two ways of defining
the same characteristics. That is, if you do not know the contact resistance, you can define the thin
material and its thickness and have the solver derive the resistance.
•
Side Dependent
The boundary condition details are set independently on each side of the domain interface. When
the domain interface is created, new boundaries are added to the Outline tree. You will have to
edit those boundaries manually.
13.1.3.1.1. Conservative Interface Flux: Interface Model
13.1.3.1.1.1. None
No models are provided for any additional heat transfer between side 1 and side 2 of the interface.
13.1.3.1.1.2. Interface Model Option: Thermal Contact Resistance
Enter a numerical quantity or CEL expression that specifies the value of the thermal contact resistance
from side 1 to side 2 of the interface.
13.1.3.1.1.3. Interface Model Option: Thin Material
Select a material and enter a numerical quantity or CEL expression that specifies the value of the
thickness of the material spanning from side 1 to side 2 of the interface.
13.1.3.1.2. Side Dependent
Side Dependent has no suboptions.
13.1.3.2. Additional Variable
Determines whether or not additional variable models are applied between the sides of the interface.
144
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Domain Interface
The options are:
•
Conservative Interface Flux
•
Side Dependent
13.1.3.2.1. Conservative Interface Flux: Interface Model
13.1.3.2.1.1. None
No models are provided for the Additional Variable between side 1 and side 2 of the interface.
13.1.3.2.1.2. Interface Model Option: Additional Variable Contact Resistance
Enter a numerical quantity or CEL expression that specifies the value of the Additional Variable contact
resistance from side 1 to side 2 of the interface.
13.1.3.2.2. Side Dependent
Side Dependent has no suboptions.
13.1.4. Domain Interface: Mesh Connection Tab
The Mesh Connection tab contains the following groups of settings:
•
Mesh Connection Method (p. 145)
13.1.4.1. Mesh Connection Method
You must specify a mesh connection method for all interface models.
13.1.4.1.1. Mesh Connection: Option
The following options may be available, depending on other settings:
•
Automatic
•
1:1 Direct (One-to-One)
•
GGI (General Grid Interface)
For details on these options, see Mesh Connection Options in the CFX-Solver Modeling Guide.
13.1.4.1.2. Intersection Control
You can use the options described in this section to control the intersection of non-matching meshes
for a particular interface.
Note
You can also use Solver Controls to apply default controls for the intersection of all interfaces
(settings which are overwritten by Intersection Control settings that you apply individually
to domain interfaces using the settings below). See Intersection Control (p. 209) to learn how
to apply default Intersection Control settings to all interfaces.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
145
Chapter 13: Domain Interfaces
Note
•
If Direct (one-to-one) mesh connectivity is available, the solver will ignore the Intersection
Control option and will instead use a 'topological intersection', that is, use the one-to-one
information to generate the intersection data.
•
If you are restarting a run, the intersection step is skipped and the intersection data is read
from the results file. This behavior can be overridden by setting the expert parameter force
intersection to True.
13.1.4.1.2.1. Intersection Control: Option
The Intersection Control options for when the Mesh Connection Option is set to GGI or Automatic
are as described below. The following options can be used to control the intersection of non-matching
meshes. CFX provides the GGI (General Grid Interface) capability which determines the connectivity
between the meshes on either side of the interface using an intersection algorithm. In general, two intersection methods are provided:
•
Bitmap Intersection:
Two faces on either side of the interface which have to be intersected are both drawn into an
equidistant 2D pixel map. The area fractions are determined by counting the number of pixels
which reside inside both intersected faces (that is, within the union of the two faces). The area
fraction for a face is then calculated by dividing the number of overlapping pixels by the total
number of pixels in the face. This method is very robust.
•
Direct Intersection (Default):
Two faces on either side of the interface are intersected using the Sutherland-Hodgeman clipping
algorithm. This method computes the exact area fractions using polygon intersection, and is much
faster and more accurate than the bitmap method.
The Bitmap Resolution controls the number of pixels used to fill the 2D pixel map (see description of
the bitmap intersection method above). The higher this number, the more accurate the final calculation
of the area fractions. In general, the default resolution of 100 should be sufficient but large differences
in the mesh resolution on both sides of the interface as well as other mesh anomalies may require the
bitmap resolution to be increased. Larger numbers will cause longer intersection times, for example,
doubling the bitmap resolution will approximately quadruple the GGI intersection time.
Both Intersection Control options enable you to set the following:
Permit No Intersection
When the Permit No Intersection option is set, the solver will run when there is no overlap between
the two sides of an interface. This parameter is mainly useful for transient cases where interface geometry
is closing and opening during the run. For example, transient rotor-stator cases with rotating valves, or
moving mesh cases where the GGI interface changes from overlap to non-overlap during the simulation
both can exhibit this type of behavior. This parameter is not switched on by default.
Discernible Fraction
Controls the minimum area fraction below which partially intersected faces are discarded. The following
default values used by the solver depend on the intersection method:
146
•
Bitmap Intersection: 1/(Bitmap Resolution)^1.5
•
Direct Intersection: 1.0E-06
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Domain Interface
Edge Scale Factor
Controls the value of the GGI edge scale factor. Control volume sector faces on GGI interfaces are detected
as degenerate if two opposite edges are smaller than the GGI edge scale factor times the cube root of
the corresponding sector volume. Those faces are not intersected.
Periodic Axial Radial Tolerance
Used when determining if the surface represented by the interface is a constant axial or radial surface.
For a rotational periodic GGI interface, the solver ensures that the ratio of the radial and axial extent
compared to the overall extent of each interface side is bigger than the specified value and therefore,
the interface vertices do not have the same radial or axial positions.
Circumferential Normalized Coordinates Option
The Circumferential Normalized Coordinates Option is used to set the type of normalization applied
to the axial or radial position coordinates (η). Mesh coordinate positions on GGI interfaces using pitch
change are transformed into a circumferential (θ) and axial or radial position (η). The η coordinates span
from hub to shroud and are normalized to values between 0 and 1. In cases where the hub and/or
shroud curves do not match on side 1 and side 2, different approaches are available to calculate the
normalized η coordinates based on side local or global minimum and maximum η values:
•
Mixed (Default for Fluid Fluid interfaces): Normalization of η is based on local minimum and maximum
η values as well as the η range of side 1. This method forces the hub curves on side 1 and 2 to align.
Non-overlap regions adjacent to the shroud may be produced if the shroud curves are not the same.
•
Global (Default for Fluid Solid Interfaces): Normalization of η is based on global minimum and
maximum eta values. This method intersects side 1 and 2 unchanged from their relative positions
in physical coordinates. If the hub and shroud curves do not match then non-overlap regions will
be produced.
•
Local: Normalization of η is done locally for each side of the interface. This method will always
produce an intersection of side 1 and 2, but may cause undesirable scaling of the geometry in some
cases.
Face Search Tolerance Factor
A scaling factor applied to the element sized based separation distance, which is used to find candidates
for intersection. For a given face on side 1 of the interface, candidate faces for intersection are identified
on side 2 using an octree search algorithm. The octree search uses this tolerance to increase the sizes
of the bounding boxes used to identify candidates. Making this parameter larger will increase the size
of the bounding boxes, resulting in possible identification of more candidates.
Face Intersection Depth Factor
A scaling factor applied to the element sized based separation distance used when performing the direct
or bitmap intersection. The final intersection of faces is only applied to those faces which are closer to
each other than a specified distance. This distance is calculated as the sum of the average depth of the
elements on side 1 and side 2 of the interface. This factor is applied as a scaling on the default distance.
It might be necessary to adjust this factor if the normal element depth on the two interfaces sides varies
a lot, or side 1 and 2 of the interface are separated by thin regions (for example, thin fin type geometries).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
147
148
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 14: Boundary Conditions
Boundary conditions must be applied to all the bounding regions of your domains. Boundary conditions
can be inlets, outlets, openings, walls, and symmetry planes.
Unspecified external regions are automatically assigned a no-slip, adiabatic wall boundary condition.
Such regions assume the name <Domain> Default, where <Domain> corresponds to the name of
the domain. Unspecified internal boundaries are ignored.
You can apply boundary conditions to any bounding surface of a 3D primitive that is included in a domain
(including internal surfaces). If you choose to specify a boundary condition on an internal surface (for
example, to create a thin surface), then boundary conditions must be applied to both sides of the surface.
This chapter describes:
14.1. Default Boundary Condition
14.2. Creating and Editing a Boundary Condition
14.3. Interface Boundary Conditions
14.4. Symmetry Boundary Conditions
14.5. Working with Boundary Conditions
Additional information on boundary conditions is available in:
•
The Purpose of Boundary Conditions in the CFX-Solver Modeling Guide
•
Available Boundary Conditions in the CFX-Solver Modeling Guide
•
Using Boundary Conditions in the CFX-Solver Modeling Guide
14.1. Default Boundary Condition
You should be familiar with the concept of primitive and composite regions before reading this section.
If you are not, see Mesh Topology in CFX-Pre (p. 91) for details.
When a domain is created, all of the bounding 2D regions that are not used elsewhere are assigned to
a default boundary condition that is created automatically. These regions can be considered to be the
boundary between the current domain and the rest of the "world". The boundary that is generated is
given the name <Domain name> Default. When 2D primitives (or composites that reference them)
are assigned to other boundary conditions and domain interfaces, they are removed from the <Domain
name> Default boundary condition. The default boundary condition is a no-slip adiabatic wall, but
this can be edited like any other boundary condition. Solid-world 2D primitives behave in a similar way.
Removing Regions from the Default Domain
Fluid-solid regions are initially contained in the <Domain Name> Default boundary condition.
When a CFX-Solver input file is written, or a user-defined domain interface is created, any fluid-solid
regions referenced by this interface are removed from the default boundary.
If every region is assigned to another boundary condition, the <Domain Name> Default boundary
object will cease to exist. In such a case, if a boundary condition is subsequently deleted, the <Domain
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
149
Chapter 14: Boundary Conditions
name> Default wall boundary will be recreated for the unspecified region. Because the <Domain
name> Default wall boundary condition is controlled automatically, you should never need to explicitly
edit its Location list.
Internal 2D Regions
Any 2D regions that lie within a domain are ignored unless a boundary condition is explicitly assigned
(these are treated as thin surfaces). Each side of a fluid-fluid 2D primitive can have a different boundary
condition, but most often both sides will be a wall. Thin surfaces are created by assigning a wall
boundary condition to each side of a fluid-fluid 2D region. You can specify physics (such as thermal
conduction) across thin surfaces in CFX-Pre by defining a domain interface. For details, see Defining
Domain Interfaces as Thin Surfaces in the CFX-Solver Modeling Guide.
14.2. Creating and Editing a Boundary Condition
To create a new boundary:
on the main toolbar.
1.
Select Insert > Boundary from the main menu or by clicking Boundary
2.
Enter a new name, if required, using the rules described in Valid Syntax for Named Objects (p. 55) and
click Apply.
To edit an existing boundary:
1.
Right-click the boundary's name in the Outline view.
2.
Select Edit. The details view for the boundary appears.
For more information on the edit command, see Outline Tree View (p. 5).
The details view describes the characteristics of a boundary condition on a series of tabs:
•
Boundary Basic Settings Tab (p. 150)
•
Boundary Details Tab (p. 152)
•
Boundary Fluid Values Tab (p. 157)
•
Boundary Sources Tab (p. 163)
•
Boundary Plot Options Tab (p. 163)
14.2.1. Boundary Basic Settings Tab
This tab sets the type, location, coordinate frame, and frame type (stationary or rotating) for each
boundary condition as detailed in the following sections:
•
Boundary Type (p. 151)
•
Location (p. 151)
•
Coord Frame (p. 151)
•
Frame Type (p. 151)
•
Profile Boundary Conditions (p. 151)
150
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
14.2.1.1. Boundary Type
Inlet, outlet, opening, wall, and symmetry boundary conditions can be selected. Interface boundaries can
be edited, but not created. For details, see Available Boundary Conditions in the CFX-Solver Modeling
Guide.
14.2.1.2. Location
You can choose the location of a boundary condition from a list containing all 2D composite and
primitive regions. For details, refer to the following sections:
•
Mesh Topology in CFX-Pre (p. 91)
•
Boundary Condition and Domain Interface Locations (p. 93)
The drop-down list contains commonly used regions (all composite names and primitive names that
are not referenced by any composites) and the extended list (displayed when clicking the Ellipsis icon
) contains all regions in a domain.
Tip
•
Hold the Ctrl key as you click to select multiple regions.
•
With the Location drop-down list active, you can select regions by clicking them in the
viewer with the mouse. This will display a small box containing the names of the regions
that are available for selection.
14.2.1.3. Coord Frame
Coordinate frames are used to determine the principal reference directions of specified and solved
vector quantities in your domain, and to specify reference directions when creating boundary conditions
or setting initial values. By default, CFX-Pre uses Coord 0 as the reference coordinate frame for all
specifications in the model, but this can be changed to any valid CFX-Pre coordinate frame. For details,
see Coordinate Frames (p. 255) and Coordinate Frames in the CFX-Solver Modeling Guide.
14.2.1.4. Frame Type
When the boundary condition is in a rotating domain, the Frame Type setting affects whether the
conditions you specify on the boundary (pressure, velocity, and so on) are interpreted relative to the
(rotating) domain (Frame Type set to Rotating) or relative to the absolute (stationary) frame of reference (Frame Type set to Stationary), from the point of view of absolute versus relative quantities.
For details, refer to the following sections:
•
Cartesian Velocity Components in the CFX-Solver Modeling Guide
•
Cylindrical Velocity Components
14.2.1.5. Profile Boundary Conditions
This option is available only if profile data is loaded.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
151
Chapter 14: Boundary Conditions
14.2.1.5.1. Use Profile Data
Select Use Profile Data to define this boundary condition using an external profile data file, rather than
using a value or expression. In order to do this, it is necessary to load the profile data file into CFX-Pre.
14.2.1.5.1.1. Initializing Profile Data
1.
Select Tools > Initialize Profile Data.
The Initialize Profile Data dialog box appears
2.
Click Browse.
3.
Select the file containing your profile data.
4.
Click Open. The profile data is loaded and the profile data name, coordinates, variable names and
units are displayed.
Note that if the path or filename are altered by typing in Data File the OK and Apply buttons
will become unavailable. You must then click Reload to read the specified file and update the
contents in the displayed profile data information.
5.
Click OK.
Under the library section of the object tree, a new User Function object is generated for this
profile function.
14.2.1.5.1.2. Profile Boundary Setup
Choose from the Profile Name list and click Generate Values to apply.
14.2.2. Boundary Details Tab
Boundary value settings depend on characteristics of the flow. For instance, temperature is required at
a boundary only if heat transfer is being modeled.
If you are changing the characteristics of the flow, ensure that boundary conditions are correctly updated.
In most cases, CFX-Pre alerts you of the need to update settings in the form of physics validation errors.
For details, see Physics Message Window (p. 11).
Example:
Suppose a domain is created, isothermal flow is specified, and an inlet boundary condition set. If flow
characteristics are then altered to include heat transfer, the inlet specification must be changed to include
the temperature of the fluid at that location.
More information on some of the settings is available:
•
Mass and Momentum in the CFX-Solver Modeling Guide
•
Flow Direction in the CFX-Solver Modeling Guide
•
Turbulence in the CFX-Solver Modeling Guide
•
Heat Transfer in the CFX-Solver Modeling Guide
•
Mesh Deformation in the CFX-Solver Modeling Guide
Various settings are available on the Boundary Details tab, depending on the type of boundary condition:
152
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
•
Boundary Details: Inlet (p. 153)
•
Boundary Details: Outlet (p. 153)
•
Boundary Details: Opening (p. 154)
•
Boundary Details: Wall (p. 154)
•
Boundary Details: Symmetry (p. 156)
•
Boundary Details: Interfaces (p. 156)
14.2.2.1. Boundary Details: Inlet
14.2.2.1.1. Flow Regime: Inlet
Option can be set to one of Subsonic, Supersonic, or Mixed. For details, refer to the following
sections:
•
Inlet (Subsonic) in the CFX-Solver Modeling Guide
•
Inlet (Supersonic) in the CFX-Solver Modeling Guide
•
Inlet (Mixed Subsonic-Supersonic) in the CFX-Solver Modeling Guide
14.2.2.1.2. Mesh Motion: Inlet
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in
the CFX-Solver Modeling Guide.
14.2.2.2. Boundary Details: Outlet
14.2.2.2.1. Flow Regime: Outlet
First, specify the flow regime option. For details, refer to the following sections:
•
Outlet (Subsonic) in the CFX-Solver Theory Guide
•
Outlet (Supersonic) in the CFX-Solver Theory Guide
14.2.2.2.2. Mass and Momentum: Outlet
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
14.2.2.2.3. Pressure Averaging: Outlet
This option appears when Average Static Pressure is selected under Mass and Momentum.
For details, see Average Static Pressure in the CFX-Solver Modeling Guide.
14.2.2.2.4. Thermal Radiation: Outlet
For details, see Thermal Radiation in the CFX-Solver Modeling Guide.
14.2.2.2.5. Mesh Motion: Outlet
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in
the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
153
Chapter 14: Boundary Conditions
14.2.2.3. Boundary Details: Opening
14.2.2.3.1. Mass and Momentum: Opening
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
14.2.2.3.2. Flow Direction: Opening
This option appears when a flow direction is required; that is, when one of Opening Pres. and
Dirn. or Static Pres. and Dirn. is selected under Mass and Momentum. For details, see
Flow Direction in the CFX-Solver Modeling Guide.
14.2.2.3.3. Loss Coefficient: Opening
For details, see Loss Coefficient in the CFX-Solver Modeling Guide
14.2.2.3.4. Turbulence: Opening
For details, see Turbulence in the CFX-Solver Modeling Guide.
14.2.2.3.5. Heat Transfer: Opening
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
14.2.2.3.6. Thermal Radiation: Opening
This is the same as specifying thermal radiation at an inlet. For details, see Thermal Radiation in the
CFX-Solver Modeling Guide.
14.2.2.3.7. Component Details: Opening
The Component Details section appears when a variable composition/reacting mixture has been created
for a single phase simulation, or a simulation with one continuous phase and particle tracking.
The mass fractions must sum to unity on all boundaries. With this in mind, highlight the materials you
want to modify and enter the mass fraction. To enter an expression for the mass fraction, click Enter
Expression
and enter the name of your expression.
14.2.2.3.8. Mesh Motion: Opening
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in
the CFX-Solver Modeling Guide.
14.2.2.4. Boundary Details: Wall
14.2.2.4.1. Mass And Momentum
Option can be set to one of No Slip Wall, Free Slip Wall, Finite Slip Wall, Specified
Shear, Counter-rotating Wall, Rotating Wall or Fluid Dependent. For details, see Mass
and Momentum in the CFX-Solver Modeling Guide.
154
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
14.2.2.4.1.1. Slip Model Settings
The Slip Model settings apply for finite slip walls.
The only available option is Power Law. You must provide the nominal slip speed (Us), the critical
stress ( ), the slip power (m), the pressure coefficient (B), and the normalizing stress ( ).
For details about the finite slip wall model, see Finite Slip Wall in the CFX-Solver Modeling Guide.
14.2.2.4.1.2. Shear Stress Settings
The Shear Stress settings apply for walls with specified shear.
You specify the shear stress value directly, using a vector that points tangentially to the wall. The normal
component of the vector that you specify is ignored.
14.2.2.4.1.3. Wall Velocity Settings
The Wall Velocity settings apply for no slip walls, and walls with finite slip.
If Wall Velocity > Option is set to Cartesian Components, you must specify the velocity in the X,
Y, and Z-axis directions. Similarly, if you choose Cylindrical Components then values are required
for Axial Component, Radial Component, and Theta Component.
Specifying a Rotating Wall requires an angular velocity and, if the domain is stationary, an axis
definition.
14.2.2.4.1.3.1. Axis Definition
If you select Coordinate Axis, a Rotation Axis is required. The Two Points method requires a
pair of coordinate values specified as Rotation Axis From and Rotation Axis To.
14.2.2.4.2. Wall Roughness
For details, see Wall Roughness in the CFX-Solver Modeling Guide.
14.2.2.4.3. Solid Motion: Wall
If the boundary is for a domain that involves solid motion, then the Solid Motion > Boundary Advection
option may be available. If the velocity for the solid motion (specified in the Boundary Details tab for
the domain) is directed into the domain everywhere on a boundary, and if you specify a fixed temperature or a fixed value of an Additional Variable on that boundary, then you should consider turning on
the Boundary Advection option.
If you have specified a fixed temperature, then turning on the Boundary Advection option causes the
advection of thermal energy into the solid domain at a rate that is consistent with the velocity normal
to the boundary, the specified fixed temperature, and the material properties.
If you have specified a fixed value for an Additional Variable, then turning on the Boundary Advection
option causes the advection of that Additional Variable into the solid domain at a rate that is in accordance with the velocity normal to the boundary, the specified fixed value of the Additional Variable, and,
for mass-specific Additional Variables, the density of the solid material.
For a boundary where the solid is moving out of the domain, consider turning on the Boundary Advection option in order to allow thermal energy and Additional Variables to be advected out.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
155
Chapter 14: Boundary Conditions
For details on setting up the solid motion model for a domain, see Solid Motion (p. 128). For details on
Additional Variables, see Additional Variables (p. 275).
14.2.2.4.4. Heat Transfer: Wall
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
14.2.2.4.5. Thermal Radiation: Wall
For details, see Thermal Radiation in the CFX-Solver Modeling Guide.
14.2.2.4.6. Mesh Motion: Wall
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Motion in the
CFX-Solver Modeling Guide.
14.2.2.4.7. Additional Coupling Sent Data
This setting is available for ANSYS Multi-field runs. For details, see Additional Coupling Sent Data in the
CFX-Solver Modeling Guide.
14.2.2.5. Boundary Details: Symmetry
Only Mesh Motion can be set in this tab for Symmetry boundary conditions. The option for Mesh
Motion is set to Unspecified by default. For details, see Mesh Deformation in the CFX-Solver Modeling
Guide.
14.2.2.6. Boundary Details: Interfaces
The options for Mass and Momentum, Turbulence, Heat transfer, Mesh Motion, and Additional
Variables are set to Conservative Interface Flux by default.
Important
Conservative Interface Flux implies that the quantity in question will “flow”
between the current boundary and the boundary on the other side of the interface. This
means that Conservative Interface Flux must also be used on the boundary on
the other side of the interface. Accordingly, the CFX-Solver will not be able to handle cases
where Conservative Interface Flux is set on just one side of the interface, or where
the quantity being transferred does not exist on the other side. CFX-Pre will issue a warning
if either of these cases exist.
For details on Nonoverlap Conditions, refer to Non-overlap Boundary Conditions.
14.2.2.7. Mesh Motion
When mesh deformation is selected for the domain that contains a boundary condition, mesh motion
can be specified for the boundary on the Boundary Details tab.
The available options are:
•
Conservative Interface Flux
•
Unspecified
156
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
•
Stationary
•
Specified Displacement
•
Specified Location
•
ANSYS MultiField
•
Rigid Body Solution
For details on these options, see Mesh Motion Options in the CFX-Solver Modeling Guide.
For details on mesh deformation, see Mesh Deformation in the CFX-Solver Modeling Guide.
See Mesh Deformation (p. 113) for information about activating mesh deformation for the domain.
14.2.3. Boundary Fluid Values Tab
The Fluid Values tab for a boundary condition object is used to set boundary conditions for each fluid
in an Eulerian multiphase simulation and each particle material when particle tracking is modeled.
The Boundary Conditions list box contains the materials of the fluid passing through the boundary
condition. Selecting a material from the list will create a frame with the name of the material and
properties available to edit. These properties are detailed in the following sections.
14.2.3.1. Fluid Values: Turbulence
Turbulence > Option can be set to any one of the following values. Unless otherwise specified, do not
change any further turbulence settings.
•
Low (Intensity = 1%)
•
Medium (Intensity = 5%)
•
High (Intensity = 10%)
•
Intensity and Length Scale
For details, see Intensity and Length Scale (p. 158).
•
Intensity and Eddy Viscosity Ratio
For details, see Intensity and Eddy Viscosity Ratio (p. 158).
•
k and Epsilon
For details, see k and Epsilon (p. 158).
•
k and Omega
•
k and Eddy Viscosity Ratio
•
k and Length Scale
•
Reynolds Stresses and Epsilon
•
Reynolds Stresses and Omega
•
Reynolds Stresses and Eddy Viscosity Ratio
•
Reynolds Stresses and Length Scale
•
Default Intensity and Autocompute Length Scale
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
157
Chapter 14: Boundary Conditions
•
Intensity and Autocompute Length
For details, see Intensity and Auto Compute Length (p. 158).
•
Zero Gradient
14.2.3.1.1. Intensity and Length Scale
Enter a numeric value or an expression for Value, and specify a value for the eddy length scale.
14.2.3.1.2. Intensity and Eddy Viscosity Ratio
Enter a numeric value or an expression for Value, and specify a value for the eddy viscosity ratio.
14.2.3.1.3. k and Epsilon
Specify a turbulent kinetic energy value and a turbulent eddy dissipation value.
14.2.3.1.4. Intensity and Auto Compute Length
Enter a numeric value or an expression for Value.
14.2.3.2. Fluid Values: Volume Fraction
Volume Fraction > Option can be set to:
•
Value
If set to Value, you must enter a numeric value or an expression for the volume fraction for each
fluid. Note that the total volume fractions of the fluids in the list box must be equal to 1.
•
Zero Gradient
The volume fraction can also be set to Zero Gradient, which implies that the volume fraction
gradient perpendicular to the boundary is zero. This setting can be useful for subcritical free surface
flow when the free surface elevation is specified (via a pressure profile) at the outlet.
14.2.3.3. Fluid Values: Heat Transfer
If Option is set to Static Temperature, you must specify a value for the static temperature.
If Option is set to ANSYS MultiField, then only the data to Receive from ANSYS can be specified.
While data can be received from ANSYS on a fluid specific basis, data can not be sent to ANSYS on that
basis (that is, multiple CFX values sent to the same receiving value in ANSYS). To send data to ANSYS,
create an Additional Coupling Sent Data object on the Boundary Details tab. For details, see Additional Coupling Sent Data in the CFX-Solver Modeling Guide.
14.2.3.4. Fluid Values for Inlets and Openings
14.2.3.4.1. Multiphase
1.
Set the fluid velocity on the Boundary Details tab.
2.
Select from the following:
•
158
Normal Speed
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
•
Cartesian Velocity Components
•
Mass Flow Rate
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
3.
Set the static pressure on the Boundary Details tab.
4.
Select from the following:
•
Normal to Boundary
•
Directional Components
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
5.
Set turbulence quantities at the inlet boundary (if applicable).
For details, see Turbulence in the CFX-Solver Modeling Guide.
6.
Set the inlet temperature of each phase (if applicable).
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
7.
Enter the volume fraction of the selected fluid at the inlet.
The total volume fraction summed over all the fluids must be equal to 1.
8.
If one of the fluids is a variable composition mixture, specify the mass fractions of each of the components.
For details, see Component Details: Opening (p. 154).
14.2.3.4.2. MUSIG settings
When the fluid selected in the list box at the top of the Fluid Values tab has a morphology of Polydispersed Fluid, size fractions must be specified for each of the size groups. The size fractions
can be set to Value or Automatic. All size fractions set to Automatic are calculated to have the
same value such that the overall sum of size fractions (including those that are specified by value) is
unity. If all size fractions are set to Value, you must ensure that the specified size fractions sum to
unity.
14.2.3.4.3. Particle Tracking Settings for Inlets and Openings
14.2.3.4.3.1. Phase List
Select the phase for which to set properties.
14.2.3.4.3.2. Particle Behavior
Optionally, specify particle properties at the boundary.
When this check box is disabled, particles do not enter through this boundary.
14.2.3.4.3.3. Mass and Momentum
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
159
Chapter 14: Boundary Conditions
14.2.3.4.3.4. Particle Position
For details, see Particle Position in the CFX-Solver Modeling Guide.
14.2.3.4.3.5. Particle Locations
For details, see Particle Locations in the CFX-Solver Modeling Guide.
14.2.3.4.3.6. Number of Positions
Select from Direct Specification or Proportional to Mass Flow Rate. For details, see
Number of Positions in the CFX-Solver Modeling Guide.
14.2.3.4.3.7. Particle Mass Flow
For details, see Particle Mass Flow Rate in the CFX-Solver Modeling Guide.
14.2.3.4.3.8. Particle Diameter Distribution
For details, see Particle Diameter Distribution in the CFX-Solver Modeling Guide.
14.2.3.4.3.9. Heat Transfer
Available when heat transfer is selected. For details, see Heat Transfer in the CFX-Solver Modeling Guide.
14.2.3.4.3.10. Component Details
Available when the particle phase has been set up as a variable composition mixture. For details, see
Component Details in the CFX-Solver Modeling Guide.
14.2.3.5. Fluid Values for Outlets
If you are using the inhomogeneous multiphase model and have selected the Fluid Velocity option
on the Boundary Details tab, the fluid-specific velocity information is set on the tab shown below at
an outlet boundary.
Specify the Mass and Momentum as:
•
Normal Speed
•
Cartesian Velocity Components
•
Cylindrical Velocity Components
•
Mass Flow Rate
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
14.2.3.6. Fluid Values for Walls
14.2.3.6.1. Particle Tracking Settings for Walls
This tab enables you to define particle behavior at walls. This is done by selecting a particle type from
the list box and specifying its properties as outlined below:
•
160
Select a particle-wall interaction option - for details, see Settings for Particle-Wall Interaction (p. 161).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating and Editing a Boundary Condition
•
Specify an erosion model - for details, see Erosion Model in the CFX-Solver Modeling Guide.
•
Specify a particle-rough wall model - for details see Particle-Rough Wall Model (Virtual Wall Model) in
the CFX-Solver Modeling Guide.
•
Specify the amount of mass absorbed at a wall - for details, see Mass Flow Absorption in the CFX-Solver
Modeling Guide.
•
Define the particle behavior - Select this option to control the entry of particles and to specify particle
properties at wall boundaries. The settings for this option are similar to those available for inlets and
openings. For details, see Particle Tracking Settings for Inlets and Openings (p. 159).
14.2.3.6.2. Settings for Particle-Wall Interaction
The particle-wall interaction can be controlled by selecting one of the following Wall Interaction options:
•
Equation Dependent - This is the default option in ANSYS CFX and requires the specification of
the following Velocity settings:
–
Restitution Coefficient - The droplet reflection at the wall can be controlled by specifying
the values for Perpendicular Coefficient and Parallel Coefficient.
The impact of droplet collision and the resulting momentum change across the collision can
be described by specifying the perpendicular and parallel coefficients of restitution. For details,
see Restitution Coefficients for Particles in the CFX-Solver Modeling Guide.
–
•
Minimum Impact Angle - Select this check box if you want to specify the minimum impact angle.
Below this impact angle, particles will be stopped with the fate Sliding along walls.
Wall Film - When Wall Interaction is set to Wall Film, then the following Wall Film Interaction
models can be selected:
–
Stick to Wall - This model enforces all particles that hit a wall to become part of the wall film.
This option does not require any further settings.
–
Elsaesser - This model requires the specification of Wall Material.
–
User Defined - The settings for this option are similar to those described for User Wall Interaction.
For details on various wall interaction options, see Wall Interaction in the CFX-Solver Modeling Guide.
User Wall Interaction - This option is available when a Particle User Routine has been created. For
details, refer to the following sections:
•
Particle User Routines (p. 295)
•
Wall Interaction in the CFX-Solver Modeling Guide
For additional modeling information on particle transport, see Particle Transport Modeling in the CFXSolver Modeling Guide.
14.2.3.7. Fluid Values for Interfaces
14.2.3.7.1. Fluid-Solid Interface, Fluid Side
The Fluid Values tab is available on the fluid side of a fluid-solid interface for an inhomogeneous
multiphase setup.
When you are using the inhomogeneous multiphase model, you must use a no-slip wall or set a wall
velocity. For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
161
Chapter 14: Boundary Conditions
When particle transport is selected, additional settings are available. These contain the same options
as those that appear for wall boundaries. For details, refer to the following sections:
•
Restitution Coefficients for Particles in the CFX-Solver Modeling Guide
•
Erosion Model in the CFX-Solver Modeling Guide
•
Mass Flow Absorption in the CFX-Solver Modeling Guide.
Particles are introduced into the domain from this boundary. For details, see Fluid Values for Inlets and
Openings (p. 158).
14.2.3.7.2. Fluid-Fluid and Periodic Interfaces
For periodic and fluid-fluid interfaces, Conservative Interface Flux is the only available option
for all quantities and cannot be changed.
14.2.4. Boundary Solid Values Tab
14.2.4.1. Heat Transfer
14.2.4.1.1. Adiabatic
The heat flux across the boundary is zero. The boundary is insulated.
14.2.4.1.2. Fixed Temperature
The boundary is fixed at a specified temperature Tw.
14.2.4.1.3. Heat Flux
A heat flux is specified across the boundary. A positive value indicates heat flux into the domain.
14.2.4.1.4. Heat Transfer Coefficient
In this case, the heat flux at a boundary is implicitly specified using an external heat transfer coefficient,
hc, and an outside or external boundary temperature, To. This boundary condition can be used to
model thermal resistance outside the computational domain. The heat flux, when calculated using the
Heat Transfer Coefficient, is:
= − (14–1)
where To is the specified outside or external boundary temperature and Tw is the temperature at the
boundary (edge of the domain).
14.2.4.1.5. Conservative Interface Flux
Conservative Interface Flux implies that the heat flow in question will be between the current
solid on this boundary and another solid on the other side of the interface. This means that Conservative Interface Flux must also be used on the boundary on the other side of the interface.
Accordingly, the CFX-Solver will not be able to handle cases where Conservative Interface
Flux is set on just one side of the interface, or where the quantity being transferred does not exist on
the other side. CFX-Pre will issue a warning if either of these cases exist.
162
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Interface Boundary Conditions
14.2.4.2. Additional Variables
See Boundary Details and Fluid Values Tabs for Boundary Condition Objects for details.
14.2.5. Boundary Sources Tab
Boundary sources of mass (continuity), energy, radiation, Additional Variables, component mass fractions,
and turbulence can be specified at inlet, opening, outlet, interface, and wall boundaries. For details, see
Sources in the CFX-Solver Modeling Guide.
Selecting Boundary Source > Sources enables you to specify sources for this boundary. For more information about sources, see Sources.
14.2.6. Boundary Plot Options Tab
The Plot Options tab enables you to create Boundary Contour and Boundary Vector graphics to
display scalar and vector values at boundaries, respectively, as detailed in the following sections:
•
Boundary Contour (p. 163)
•
Boundary Vector (p. 163)
14.2.6.1. Boundary Contour
Selecting this option and choosing a Profile Variable draws the boundary surface colored by the selected
variable. The available variables depend on the settings on the Boundary Details and Sources tabs,
as applicable. A legend appears by default showing the variable plotted on the boundary with a local
range. You can clear visibility for the legend and the plots by clearing the check box next to the
boundary contour object associated with your boundary condition in the Outline tree view. You may
have to click the + sign next to the boundary condition in order to view the contour object in the
Outline tree view.
14.2.6.2. Boundary Vector
Selecting this option draws vectors at the nodes of the boundary surface, pointing in the direction
specified by the Profile Vector Component setting. The availability of vectors (and this option) depends
on the settings on the Boundary Details and Basic Settings tabs. For example, vector plots are available
if you specify Basic Settings > Boundary Type as Inlet and the Boundary Details > Mass and
Momentum option as velocity components.
14.3. Interface Boundary Conditions
All domain interfaces automatically create boundaries of type Interface that contain the regions
used in the domain interface. These boundaries are named <Domain Interface Name> Side
<Number>. For example, for a domain interface named myInterface, the related boundary conditions
would be called myInterface Side 1 and myInterface Side 2. At least one of these
boundaries will be auto-created for each domain involved in the interface. You can edit these boundaries
like any other boundary, but you cannot create new interface boundaries directly.
You will usually not need to edit an auto-generated Interface boundary, but options are available for
fluid-solid interfaces (which can be considered a special case of wall boundaries). Settings and options
available when editing interface boundaries can be configured. For details, refer to the following sections:
•
Boundary Details: Interfaces (p. 156)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
163
Chapter 14: Boundary Conditions
•
Fluid Values for Interfaces (p. 161)
14.4. Symmetry Boundary Conditions
When specifying symmetry boundary conditions, select the locations from the drop-down list box and
select the Frame Type if your domain is rotating. No further settings are required, and the same settings
apply for fluid and solid domains.
For details, see Symmetry Plane in the CFX-Solver Modeling Guide.
14.5. Working with Boundary Conditions
The topics in this section include:
•
Boundary Condition Visualization (p. 164)
•
Profile Data and CEL Functions (p. 164)
14.5.1. Boundary Condition Visualization
When you create a boundary condition in CFX-Pre, several things happen in the Viewer:
•
Symbols for the boundary conditions are displayed in the viewer, based on type. The visibility of these
symbols is determined by the Label and Marker control form. For details, see Boundary Markers and
Labels (p. 27).
•
Boundary condition symbols are shown at surface display line intersections.
•
Regions comprising the boundary condition are highlighted according to settings specified under Edit
> Options. For details, see 3D Viewer Toolbar (p. 19).
If multiple boundary conditions are defined on a region of mesh, an error appears in the physics validation window below the viewer.
Note
Inlets, outlets, and openings use arrow symbols that are locally normal to the boundary
surface, irrespective of the actual direction specified for the boundary condition. It is possible
to show arrows pointing in the specified direction by creating a Boundary Vector object. You
can optionally turn off the default arrow symbols by clearing the check boxes on Label and
Marker control form (see above). Also see Boundary Vector (p. 163) and Boundary Markers (p. 27) for more details.
When using CFX-Pre within ANSYS Workbench or with a pale viewer background color, the
colors of these symbols are black in order to make them more visible.
14.5.2. Profile Data and CEL Functions
Profile data can be used to define a boundary condition based on a distribution of appropriate values.
14.5.2.1. Types of Discrete Profiles
•
164
1D profile uses one spatial coordinate to define the data position; for example, x, y, z, or a cylindrical
value. This could be used to describe the axisymmetric flow down a cylindrical pipe (that is, the data
values for a value of ‘r’).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with Boundary Conditions
•
2D profile uses two spatial coordinates (Cartesian or polar); for example, (x, y), (x, z), (r, t), (a, t), and so
on. If you are importing the data from a 2D code on a planar boundary, you may want to use this as a
boundary condition in a 3D case in CFX.
•
3D profile uses three spatial coordinates; for example, (x, y, z) or (r, t, a). Among various uses of 3D
Profile Data are boundary conditions, spatially varying fluid properties, Additional Variables, or equation
sources.
14.5.2.2. Profile Data Format
The following is the format of the profile data file:
# Comment line
# The following section (beginning with [Name] and ending with
# [Data]) represents one profile, which can be repeated
# to define multiple profiles.
[Name]
My Boundary
[Spatial Fields]
r, theta, z
.
.
.
[Data]
X [ m ], Y [ m ], Z [ m ], Area [ m^2 ], Density [ kg m^-3 ]
-1.773e-02, -5.382e-02, 6.000e-02, 7.121e-06, 1.231e+00
-1.773e-02, -5.796e-02, 5.999e-02, 5.063e-06, 1.231e+00
.
.
.
# -------- end of first profile 'My Boundary'---------[Name]
Plane 2
.
.
.
The following is a guideline for creating profile data format:
•
The name of each locator is listed under the [Name] heading.
•
The names of the fields are case-insensitive (that is, [data] and [Data] are acceptable).
•
The names of variables used in the data fields are case sensitive.
For example, u [m] is a valid x velocity component, whereas U [m] is an unrecognized field
name. You have to map this unrecognized field name with a valid variable name when loading
into CFX-Pre. This is consistent with the use of CEL elsewhere.
•
Comments in the file are preceded by # (or ## for the CFX polyline format) and can appear anywhere
in the file.
•
Commas must separate all fields in the profile. Any trailing commas at the end of a line are ignored.
Any additional commas within a line of data will be a syntax error.
•
Blank lines are ignored and can appear anywhere in the file (except between the [<data>] and first
data line, where <data> is one of the key words in square brackets shown in the data format).
•
If any lines with text are included above the keyword [Name], a syntax error will occur. Such lines
should be preceded by # character to convert them into comments.
•
Multiple data sets are permitted within the same file by repeating the sequence of profiles; each profile
begins with keyword [Name].
•
Point coordinates and the corresponding variable values are stored in the [Data] section.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
165
Chapter 14: Boundary Conditions
•
[Spatial Fields] can contain 1, 2, or 3 values, corresponding to 1D, 2D, or 3D data.
•
The data file has a .csv extension for compatibility with other software packages.
•
When this data file is read in, it is checked for any format violations; physics errors are shown for such
situations.
Note
Files exported from CFD-Post in a user-specified coordinate system will contain a coordinate
frame ([CoordFrame]) section. The coordinate frame definition is written to the profile
file; CFX-Pre will define that coordinate frame for you when you initialize the data.
Additional information on profile data is available:
•
Physics Message Window (p. 11)
•
RULES and VARIABLES Files in the CFX-Solver Manager User's Guide
•
Profile Boundary Conditions in the CFX-Solver Modeling Guide
14.5.2.3. Multiphase Boundary Condition Example
Consider a multiphase boundary condition set up using the following:
•
The profile data file has a profile named myProfile
•
One of the data fields is Temperature [K]
CFX-Pre enables a function such as myProfile.water.Temperature(x,y,z) to refer to a data
field stored in the profile. This derived value can be assigned to a parameter, such as Fixed Temperature.
The expressions that are automatically generated in CFX-Pre for profile boundaries are simply the expressions in terms of interpolation functions. Modify them in the same way as a normal CEL expression.
For example, the expression myProfile.Temperature(x,y,z) could be modified to 2*myProfile.Temperature(2x,y,z). For details, see Profile Boundary Conditions in the CFX-Solver Modeling
Guide.
166
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 15: Initialization
Initialization is the process by which all unspecified solution field values are assigned at the beginning
of a simulation. These values are commonly referred to as initial values. For steady state simulations,
they may be collectively referred to as an initial guess.
For steady state simulations, initial values can be set automatically if a good initial guess is not known
or is not required. Although accurate initial values may not always be available, a good approximation
can reduce the time to solve a steady state simulation and reduce the chance that the solution fails to
converge due to diverging residuals. The more complicated the simulation and models used, the more
important it becomes to start the solution process with sensible initial values. Advice about choosing
sensible initial values is available in Initialization Parameters in the CFX-Solver Modeling Guide.
For transient simulations, the initial values must be specified for all variables because the data describes
the state at the simulation start time.
If available, the results from a previous simulation can be used to provide the initial values. In this case,
any values chosen to be automatically set will be overridden by values from the initial values file(s). See
Reading the Initial Conditions from a File in the CFX-Solver Modeling Guide for details.
Global and domain initialization settings may be specified. Global settings apply to only those domains
that do not have their own initialization settings.
Information on modeling initial values is available in Initial Condition Modeling in the CFX-Solver Modeling Guide.
15.1. Using the User Interface
The following topics will be discussed:
•
Domain: Initialization Tab (p. 167)
•
Global Settings and Fluid Settings Tabs (p. 168)
The Global Settings and Fluid Settings tabs for the global initialization object (listed as Initialization under Simulation in the tree view) contain settings that specify how initial values are to be
determined, and, in some cases, the initial values themselves. They are accessible by clicking Global
, by selecting Insert > Global Initialization, or by editing the initialization object listed
Initialization
in the tree view under Simulation.
15.1.1. Domain: Initialization Tab
The Initialization tab for a domain contains settings that specify how initial values are to be determined,
and, in some cases, the initial values themselves. It is accessible by editing a domain object.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
167
Chapter 15: Initialization
15.1.1.1. Domain Initialization
This check box determines whether or not the domain is initialized based on its own settings or based
on global initialization settings. When this check box is selected, an interface that is essentially the same
as that for global initialization is displayed. Any initialization values defined on a per-domain basis will
override values defined at the global level. For details, see Global Settings and Fluid Settings Tabs (p. 168).
After specifying and applying domain initialization, an entry called Initialization is listed in the
tree view under the applicable domain.
15.1.2. Global Settings and Fluid Settings Tabs
When a simulation involves only one fluid, the Fluid Settings tab is not available, but then all of its
contents are added to the Global Settings tab.
15.1.2.1. Coord Frame Check Box
This check box determines whether or not a specified coordinate frame is used for interpreting initial
conditions. If the check box is not selected, the default coordinate frame, Coord 0, is used.
15.1.2.1.1. Coord Frame Check Box: Coord Frame
Select a coordinate frame to use for interpreting initial conditions. For details, see:
•
Coordinate Frames (p. 255)
•
Coordinate Frames in the CFX-Solver Modeling Guide
•
Coord Frame in the CFX-Solver Modeling Guide
15.1.2.2. Frame Type Check Box
This check box determines whether or not a specified frame type is used for interpreting initial values
of velocity. If the check box is not selected, the default frame of reference is used. The default frame
of reference is stationary or rotating, depending on whether the domain is stationary or rotating, respectively.
15.1.2.2.1. Frame Type
•
Stationary
The frame of reference used to interpret initial values of velocity is the stationary frame of reference.
For example, if the initial velocity throughout a domain is parallel to the rotation axis of the domain,
the flow will initially have no swirl in the stationary frame of reference, even if the domain is rotating.
•
Rotating
The frame of reference used to interpret initial values of velocity is that of the associated domain.
For example, if the initial velocity throughout a domain is specified as being parallel to the rotation
axis of the domain, and if the domain is rotating, the flow will have swirl in the stationary frame
of reference.
For details, see Frame Type in the CFX-Solver Modeling Guide.
15.1.2.3. Initial Conditions: Velocity Type
•
168
Cartesian
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Using the User Interface
•
Cylindrical
For details, see Velocity Type in the CFX-Solver Modeling Guide.
15.1.2.4. Initial Conditions: Cartesian Velocity Components
15.1.2.4.1. Option
•
Automatic
The initial velocity field is loaded from an initial values file, if one is available. If an initial values file
is not available, the initial velocity field is computed from built-in algorithms. For details, see
Automatic in the CFX-Solver Modeling Guide.
•
Automatic with Value
The initial velocity field is loaded from an initial values file, if one is available. If an initial values file
is not available, the initial velocity field is set to user-specified values. For details, see Automatic
with Value in the CFX-Solver Modeling Guide.
15.1.2.4.2. Velocity Scale Check Box
(applies only when Option is set to Automatic)
This check box determines whether or not a specified velocity scale is used. If the check box is not selected, a velocity scale will be calculated internally by the CFX-Solver, based on a weighted average
value of velocity over all applicable Boundary Conditions (inlets, openings and outlets). Initial guess
values that are calculated based on the internally calculated velocity scale may be unsuitable due to
the shape of your domain, or, for example, due to a small, high-speed inlet which results in an overprediction of the velocity magnitude.
15.1.2.4.2.1. Velocity Scale Check Box: Value
Enter a numerical quantity or CEL expression for the velocity scale. This is not a normalized value; it is
essentially the velocity magnitude that will be used for all applicable velocity vectors. For details, see
Velocity Scale in the CFX-Solver Modeling Guide.
15.1.2.4.3. U, V, W
(applies only when Option is set to Automatic with Value)
Enter a numerical quantity or CEL expression for each Cartesian velocity component. For details, see
Cartesian Velocity Components in the CFX-Solver Modeling Guide.
15.1.2.5. Initial Conditions: Cylindrical Velocity Components
15.1.2.5.1. Option
For details, see Option (p. 169).
15.1.2.5.2. Velocity Scale Check Box
(applies only when Option is set to Automatic)
For details, see Velocity Scale Check Box (p. 169).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
169
Chapter 15: Initialization
15.1.2.5.3. Axial Component, Radial Component, Theta Component
(applies only when Option is set to Automatic with Value)
Enter a numerical quantity or CEL expression for each cylindrical velocity component. For details, see
Cylindrical Velocity Components in the CFX-Solver Modeling Guide.
15.1.2.6. Initial Conditions: Static Pressure
15.1.2.6.1. Option
•
Automatic
The initial static pressure field is loaded from an initial values file, if one is available. If an initial
values file is not available, the initial static pressure field is computed from built-in algorithms.
•
Automatic with Value
The initial static pressure field is loaded from an initial values file, if one is available. If an initial
values file is not available, the initial static pressure field is set to user-specified values.
For details, see Static Pressure in the CFX-Solver Modeling Guide.
15.1.2.6.2. Relative Pressure
(applies only when Option is set to Automatic with Value)
Enter a numerical quantity or CEL expression for the relative pressure.
For details, see Static Pressure in the CFX-Solver Modeling Guide.
15.1.2.7. Initial Conditions: Turbulence
From Option, the various initial condition settings for turbulence are:
•
Low Intensity and Eddy Viscosity Ratio: This sets intensity to 1% and viscosity ratio
to 1.
•
Medium Intensity and Eddy Viscosity Ratio: This sets intensity to 5% and viscosity
ratio to 10.
•
High Intensity and Eddy Viscosity Ratio: This sets intensity to 10% and viscosity
ratio to 100.
•
Intensity and Eddy Viscosity Ratio: Use this option to specify fractional intensity and
eddy viscosity ratio.
•
Intensity and Length Scale: Use this option to specify fractional intensity and length
scale.
•
k and Epsilon: Use this option to specify turbulence kinetic energy and turbulence eddy dissipation.
•
k and Omega: Use this option to specify turbulence kinetic energy and turbulence eddy frequency.
•
k and Eddy Viscosity Ratio: Use this option to specify turbulence kinetic energy and
eddy viscosity ratio.
•
k and Length Scale: Use this option to specify turbulence kinetic energy and length scale.
170
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Using the User Interface
•
Reynolds Stresses and Epsilon: Use this option to specify Reynolds Stresses and turbulence
eddy dissipation.
•
Reynolds Stresses and Omega: Use this option to specify Reynolds Stresses and turbulence
eddy frequency.
•
Reynolds Stresses and Eddy Viscosity Ratio: Use this option to specify Reynolds
Stresses and eddy viscosity ratio.
•
Reynolds Stresses and Length Scale: Use this option to specify Reynolds Stresses and
length scale.
For additional details, see K (Turbulent Kinetic Energy), Epsilon (Turbulence Eddy Dissipation), and
Reynolds Stress Components in the CFX-Solver Modeling Guide.
15.1.2.7.1. Fractional Intensity
•
Option: Automatic
The fractional intensity field is loaded from an initial values file, if one is available. If an initial values
file is not available, the fractional intensity field is computed automatically.
•
Option: Automatic with Value
The fractional intensity field is loaded from an initial values file, if one is available. If an initial values
file is not available, the fractional intensity field is set to user-specified values.
15.1.2.7.2. Eddy Viscosity Ratio
•
Option: Automatic
The eddy viscosity ratio field is loaded from an initial values file, if one is available. If an initial values
file is not available, the eddy viscosity ratio field is computed automatically.
•
Option: Automatic with Value
The eddy viscosity ratio field is loaded from an initial values file, if one is available. If an initial values
file is not available, the eddy viscosity ratio field is set to user-specified values.
15.1.2.7.3. Eddy Length Scale
•
Option: Automatic
The eddy length scale field is loaded from an initial values file, if one is available. If an initial values
file is not available, the eddy length scale field is computed automatically.
•
Option: Automatic with Value
The eddy length scale field is loaded from an initial values file, if one is available. If an initial values
file is not available, the eddy length scale field is set to user-specified values.
15.1.2.7.4. Turbulence Kinetic Energy
•
Option: Automatic
The turbulence kinetic energy field is loaded from an initial values file, if one is available. If an initial
values file is not available, the turbulence kinetic energy field is computed automatically.
•
Option: Automatic with Value
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
171
Chapter 15: Initialization
The turbulence kinetic energy field is loaded from an initial values file, if one is available. If an initial
values file is not available, the turbulence kinetic energy field is set to user-specified values.
15.1.2.7.5. Turbulence Eddy Dissipation
•
Option: Automatic
The turbulence eddy dissipation field is loaded from an initial values file, if one is available. If an
initial values file is not available, the turbulence eddy dissipation field is computed automatically.
•
Option: Automatic with Value
The turbulence eddy dissipation field is loaded from an initial values file, if one is available. If an
initial values file is not available, the turbulence eddy dissipation field is set to user-specified values.
15.1.2.7.6. Turbulence Eddy Frequency
•
Option: Automatic
The turbulence eddy frequency field is loaded from an initial values file, if one is available. If an
initial values file is not available, the turbulence eddy frequency field is computed automatically.
•
Option: Automatic with Value
The turbulence eddy frequency field is loaded from an initial values file, if one is available. If an
initial values file is not available, the turbulence eddy frequency field is set to user-specified values.
15.1.2.7.7. Reynolds Stress Components
•
Option: Automatic
The Reynolds stress components fields are loaded from an initial values file, if one is available. If
an initial values file is not available, the Reynolds stress components fields are computed automatically.
•
Option: Automatic with Value
The Reynolds stress components fields are loaded from an initial values file, if one is available. If
an initial values file is not available, the Reynolds stress components fields are set to user-specified
values.
15.1.2.8. Initial Conditions: Temperature
(applies only when heat transfer is active)
•
Automatic
The initial temperature field is loaded from an initial values file, if one is available. If an initial values
file is not available, the initial temperature field is computed from built-in algorithms.
•
Automatic with Value
The initial temperature field is loaded from an initial values file, if one is available. If an initial values
file is not available, the initial temperature field is set to user-specified values.
172
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Using the User Interface
15.1.2.9. Initial Conditions: Radiation Intensity
(applies only when using the P1, Discrete Transfer, or Monte Carlo model for Thermal Radiation)
15.1.2.9.1. Option
•
Automatic
The initial radiation intensity field and blackbody temperature field are loaded from an initial values
file, if one is available. If an initial values file is not available, the initial radiation intensity field and
blackbody temperature field are computed from built-in algorithms.
•
Automatic with Value
The initial radiation intensity field and blackbody temperature field are loaded from an initial values
file, if one is available. If an initial values file is not available, the initial radiation intensity field and
blackbody temperature field are set to user-specified values.
For details, see Radiation Intensity in the CFX-Solver Modeling Guide.
15.1.2.10. Initial Conditions: Mixture Fraction
15.1.2.10.1. Option
•
Automatic
The initial mixture fraction field is loaded from an initial values file, if one is available. If an initial
values file is not available, the initial mixture fraction field is computed from built-in algorithms.
•
Automatic with Value
The initial mixture fraction field is loaded from an initial values file, if one is available. If an initial
values file is not available, the initial mixture fraction field is set to user-specified values.
15.1.2.10.2. Mixture Fraction
Enter a numerical quantity or CEL expression that specifies the value of the mixture fraction throughout
the domain.
15.1.2.11. Initial Conditions: Mixture Fraction Variance
15.1.2.11.1. Option
•
Automatic
The initial mixture fraction variance field is loaded from an initial values file if, one is available. If
an initial values file is not available, the initial mixture fraction variance field is computed from
built-in algorithms.
•
Automatic with Value
The initial mixture fraction variance field is loaded from an initial values file, if one is available. If
an initial values file is not available, the initial mixture fraction variance field is set to user-specified
values.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
173
Chapter 15: Initialization
15.1.2.11.2. Mix. Fracn. Variance
Enter a numerical quantity or CEL expression that specifies the value of the mixture fraction variance
throughout the domain.
15.1.2.12. Initial Conditions: Component Details
(applies only when the relevant fluid is a variable composition mixture)
15.1.2.12.1. List Box
This list box is used to select a component (of a fluid that is a variable composition mixture) in order
to set its fluid-specific initialization options.
15.1.2.12.2. [component name]: Option
•
Automatic
The initial mass fraction field is loaded from an initial values file, if one is available. If an initial values
file is not available, the initial mass fraction field is computed from built-in algorithms.
•
Automatic with Value
The initial mass fraction field is loaded from an initial values file, if one is available. If an initial values
file is not available, the initial mass fraction field is set to user-specified values.
15.1.2.12.3. [component name]: Mass Fraction
Available when Option is set to Automatic with Value, you must enter a numerical quantity or
CEL expression that specifies the value of the component mass fraction throughout the domain.
15.1.2.13. Initial Conditions: Additional Variable Details
This section is similar to Component Details, dealing with Additional Variables instead. For details, see
Initial Conditions: Component Details (p. 174).
15.1.2.14. Fluid Specific Initialization
(applies only when multiple fluids are involved)
The fluid-specific initialization settings are grouped together, either in the Fluid Specific Initialization
section or, in the case of global initialization, on the Fluid Settings tab.
15.1.2.15. Fluid Specific Initialization: List Box
This list box is used to select a fluid in order to set its fluid-specific initialization options.
15.1.2.16. Fluid Specific Initialization: [fluid name] Check Box
This check box determines whether or not the initialization options for the indicated fluid are specified
explicitly or are left at default values.
174
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Using the User Interface
15.1.2.17. Fluid Specific Initialization: [fluid name] Check Box: Initial Conditions
Most of the fluid-specific initial condition settings are described in this section as they appear in the
non-fluid specific initial condition section in the case of a single-fluid simulation. Those that are not are
described here.
15.1.2.17.1. Velocity Type
The velocity type can be either Cartesian or Cylindrical. For details, see Velocity Type in the
CFX-Solver Modeling Guide.
15.1.2.17.2. Volume Fraction: Option
•
Automatic
The initial volume fraction field is loaded from an initial values file, if one is available. If an initial
values file is not available, the initial volume fraction field is computed from built-in algorithms.
•
Automatic with Value
The initial volume fraction field is loaded from an initial values file if one is available. If an initial
values file is not available, the initial volume fraction field is set to user-specified values.
15.1.2.17.3. Volume Fraction: Volume Fraction
Enter a numerical quantity or CEL expression that specifies the value of the volume fraction throughout
the domain. For details, see Initial Conditions for a Multiphase Simulation in the CFX-Solver Modeling
Guide.
15.1.2.18. Solid Specific Initialization
(applies only when there are solids in porous domains)
The solid-specific initialization settings are grouped together, either in the Solid Specific Initialization
section or, in the case of global initialization, on the Solid Settings tab.
15.1.2.19. Solid Specific Initialization: List Box
This list box is used to select a solid in order to set its solid-specific initialization options.
15.1.2.20. Solid Specific Initialization: [solid name] Check Box
This check box determines whether or not the initialization options for the indicated solid are specified
explicitly or are left at default values.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
175
176
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 16: Source Points
Source points are sources that act on a single mesh element. The location of the point is entered in
Cartesian coordinates, and the source is created for the element whose center is closest to the specified
point. Source points appear as red spheres in the Viewer. For a transient run or run with a moving mesh,
the closest element is identified once at the start and is used for the remainder of the run.
This chapter describes:
16.1. Basic Settings Tab
16.2. Sources Tab
16.3. Fluid Sources Tab
16.4. Sources in Solid Domains
16.5. Source Points and Mesh Deformation
Sources are specified in a way similar to subdomain sources with the exceptions that momentum and
radiation sources cannot be specified and only “Total Source” values can be entered. For details, see
Subdomains (p. 181).
The visibility of source points can be turned on and off using the check box in the tree view. For details,
see Object Visibility (p. 18) and Outline Tree View (p. 5).
Additional information on sources is available in Sources in the CFX-Solver Modeling Guide.
16.1. Basic Settings Tab
The Basic Settings tab defines the coordinate frame and the point coordinates for the source point.
1.
Enter Cartesian Coordinates for the source point.
Points entered are relative to the selected coordinate frame.
2.
Use the default coordinate frame or a user-specified coordinate frame. For details, see:
•
Coordinate Frames in the CFX-Solver Modeling Guide
•
Coordinate Frame Basic Settings Tab (p. 255).
The default coordinate frame, Coord 0, will be used as the basis for the entered Cartesian coordinates,
unless you have created your own coordinate frame and have selected it from the drop-down list.
16.2. Sources Tab
The point sources that can be set depend on the physical models used in the simulation. Sources of
mass (continuity), energy, radiation, Additional Variables, component mass fractions, and turbulence
are all possible.
16.2.1. Single-Phase Fluid Sources
1.
Select the Sources check box to specify sources for the point.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
177
Chapter 16: Source Points
2.
Select the equation source to specify.
Equation sources include other sources such as mass fraction, energy, continuity (mass), turbulence,
Additional Variables, and so on. For details, see Source Coefficient / Total Source Coefficient in
the CFX-Solver Modeling Guide.
3.
Select the Continuity check box to set sources for the continuity equation.
For details, see Mass (Continuity) Sources in the CFX-Solver Modeling Guide.
Additional information is available in:
•
Sources in the CFX-Solver Modeling Guide
•
General Sources in the CFX-Solver Modeling Guide.
16.2.1.1. Component Mass Fractions
This is only available when mixtures are included in the fluids list in the domain. You can specify a Total
Source and an optional Total Source Coefficient for improved convergence for strongly varying sources.
For details, see General Sources in the CFX-Solver Modeling Guide.
16.2.1.2. Additional Variables
Set the Total Source for the Additional Variable and an optional Total Source Coefficient. A source
for an Additional Variable can be set only if it is solved for.
16.2.1.3. Continuity
Continuity sources differ from other sources because you are introducing new fluid into the domain.
Properties that are required of the fluid, which is entering the domain, appear in the Variables section
of the form. These values are not used if the source is negative, because no new fluid is introduced into
the subdomain. For details, see Mass (Continuity) Sources in the CFX-Solver Modeling Guide.
16.2.1.3.1. Continuity Option
The value of the mass source is set using the Total Fluid Mass Source option. For details, see Mass
(Continuity) Sources in the CFX-Solver Modeling Guide.
16.2.1.3.2. Additional Variables
Set a value for any Additional Variables that are introduced with the mass source. For details, see Mass
(Continuity) Sources in the CFX-Solver Modeling Guide.
16.2.1.3.3. Component Mass Fractions
Enter mass fractions of each of the components in the mass source. For details, see Mass (Continuity)
Sources in the CFX-Solver Modeling Guide.
16.2.1.3.4. Temperature
Enter the temperature for the mass source.
178
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Sources in Solid Domains
16.2.1.3.5. Velocity
Set velocity components for the mass source.
16.2.1.4. Energy
A total source for the energy equation can be set. The optional Total Source Coefficient provides improved convergence for strongly varying sources. An energy source can set specified when the parent
domain models heat transfer using the thermal energy or total energy models.
16.2.1.5. Turbulence Eddy Dissipation or Turbulence Kinetic Energy
When the flow is turbulent, a total source for the Turbulence Eddy Dissipation or Turbulence
Kinetic Energy can specified. The optional Total Source Coefficient provides improved convergence
for strongly varying sources. For details, see General Sources in the CFX-Solver Modeling Guide.
16.2.2. Multiphase Bulk Sources
In a multiphase simulation, source terms that apply to all fluids in the simulation are set on the Sources
tab. Bulk sources take account of the volume fraction of each phase when applying the source term.
For details, see Bulk Sources in the CFX-Solver Modeling Guide.
•
Select Bulk Sources to specify bulk sources. Bulk sources apply to all fluids in a multiphase simulation.
16.2.3. Multiplying Sources by Porosity
Selecting the Multiply by Porosity check box causes the equation source to be scaled by the porosity
value. For example, if a porous domain has a volume porosity of 0.8, then if the Multiply by Porosity
check box is selected, 80% of the source is applied to the fluid; if the check box is not selected then
100% of the source is applied to the fluid.
16.3. Fluid Sources Tab
Fluid sources can be set when more than one fluid is selected. The options depend on the type of
simulation you are running, and whether bulk sources are used.
1.
Select the fluid from the Fluid Specific Source Point Sources list
2.
Select the check box next to the selected variable to enter a source, then select the Continuity check
box.
3.
Enter a value for Total Source.
4.
Optionally, enter a total mass source coefficient for either pressure or volume fraction.
For details, see Source Coefficient / Total Source Coefficient in the CFX-Solver Modeling Guide.
5.
Set the values for the continuity equation.
For details, see Mass (Continuity) Sources in the CFX-Solver Modeling Guide.
16.4. Sources in Solid Domains
Source points can exist in solid domains to provide sources of thermal energy and radiation.
•
Select Energy to enable an energy source.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
179
Chapter 16: Source Points
For details, see General Sources in the CFX-Solver Modeling Guide.
16.5. Source Points and Mesh Deformation
When mesh deformation is selected, the volume element whose centroid is closest to the source point
at the beginning of the simulation will move with the mesh (if that part of the mesh is deforming). The
location of the point source will, therefore, move as the mesh deforms. For details, see Mesh Deformation (p. 113).
180
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 17: Subdomains
A subdomain is a 3D region within a predefined domain that can be used to specify values for volumetric
sources. Fluid or porous subdomains (that is, when the parent domain is of type Fluid) allow sources
of energy, mass, momentum, radiation, Additional Variables, components, and turbulence to be specified.
Solid subdomains allow only sources of energy and radiation to be set.
This chapter describes:
•
Creating New Subdomains (p. 181)
•
The Subdomains Tab (p. 182)
•
Basic Settings Tab (p. 182)
•
Sources Tab (p. 182)
•
Fluids Tab (p. 185)
•
Mesh Motion (p. 185)
A domain must be created before a subdomain can be created. The location of a subdomain must be
a 3D region that is part of a single parent domain. 3D primitives are implicitly included in a parent domain
if 3D composites or assemblies are used in the domain location. A subdomain cannot span more than
one domain, but you can create many subdomains in each domain. You should consider subdomain
requirements when you generate a mesh, because subdomains must be created on existing 3D regions.
Definitions for primitive and composite regions are available in Mesh Topology in CFX-Pre (p. 91).
Additional information on the physical interpretation of subdomain sources and modeling advice is
available, as well as additional information on the mathematical implementation of sources, is available
in Sources in the CFX-Solver Modeling Guide.
The CFX Expression Language (CEL) can be used to define sources by creating functions of any CFX
System Variables. For details, see CEL Operators, Constants, and Expressions in the CFX Reference Guide.
17.1. Creating New Subdomains
New subdomains are created by selecting Insert > Sub Domain from the main menu or by clicking
Subdomain
on the main toolbar. Note that creation of subdomains from the main menu or toolbar
may subsequently require selection of the appropriate analysis type and domain. Subdomains can also
be created by right-clicking the appropriate domain in the Outline view.
1.
Enter a new name using the syntax described below or pick an existing subdomain to edit.
2.
Select the parent domain for the subdomain.
Additional information on valid names is available in Valid Syntax for Named Objects (p. 55). You can
also edit an existing subdomain by selecting its name from the drop-down list. Existing subdomains
can also be edited from the Outline view using the usual methods; for details, see Outline Tree
View (p. 5).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
181
Chapter 17: Subdomains
17.2. The Subdomains Tab
After entering a name for the subdomain, or selecting the subdomain to edit, the subdomain details
view will be displayed. This contains two tabs, Basic Settings and Sources, that are accessed by selecting
the tabs located across the top. You should complete each tab in turn, proceeding from left to right.
Note
Fluid sources are on their own tab.
•
Basic Settings: Sets the location and the coordinate frame for the subdomain. For details, see Basic
Settings Tab (p. 182).
•
Sources: Defines volumetric source terms in the subdomain for single-phase simulations, or volumetric
source terms that apply to all fluids in a multiphase simulation. For details, see Sources Tab (p. 182).
•
Fluid Sources: Defines volumetric source terms that apply to individual fluid in a multiphase simulation.
17.3. Basic Settings Tab
The following settings are required on the Basic Settings tab.
•
Location (p. 182)
•
Coordinate Frame (p. 182)
17.3.1. Location
Select the region name that the subdomain will occupy. The location can be defined as multiple regions,
assemblies and/or user 3D Regions. For details, see Mesh Topology in CFX-Pre (p. 91).
17.3.2. Coordinate Frame
By default, Coordinate Frame is set to Coord 0. You may use alternative coordinate frames. To create
a new coordinate frame, select Insert > Coordinate Frame from the main menu. For details, see:
•
Coordinate Frames (p. 255)
•
Coordinate Frames in the CFX-Solver Modeling Guide.
17.4. Sources Tab
The volumetric sources that can be set in a subdomain depend on the physical models used in the
simulation. Sources of mass (continuity), momentum, energy, radiation, Additional Variables, component
mass fractions, and turbulence are all possible.
17.4.1. Single-Phase Fluid Sources
In a single-phase simulation, the volumetric or total source terms are set on the Sources tab. For details,
see Sources in the CFX-Solver Modeling Guide.
1.
Select the Sources check box to specify sources for the subdomain.
2.
Select the Momentum Source/Porous Loss check box to specify a momentum source.
182
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Sources Tab
For details, see Momentum Source/Porous Loss (p. 183).
3.
Select the equation source to specify.
Equation sources include other sources such as mass fraction, energy, continuity (mass), turbulence,
Additional Variables, and so on. For details, see:
•
Equation Sources (p. 183)
•
Source Coefficient / Total Source Coefficient in the CFX-Solver Modeling Guide.
17.4.1.1. Momentum Source/Porous Loss
A source of momentum is introduced by setting X, Y and Z, or r, Theta and Axial components for the
momentum source under General Momentum Source. All three components must be set if a general
momentum source is defined. You can optionally specify a Momentum Source Coefficient to aid
convergence. When employing a cylindrical coordinate frame, you must specify an axis using a rotation
axis or two points.
In addition to specifying a general source of momentum, you can model porous loss in a flow using an
isotropic or directional loss model. In each case, the loss is specified using either linear and quadratic
coefficients, or permeability and loss coefficients. For the Directional Loss model, the loss in the
transverse direction can be set using the Loss Coefficient, which multiplies the streamwise loss
by the entered factor. When using the Directional Loss model, you must supply a streamwise direction.
The direction can be specified with Cartesian or cylindrical coordinates. If you choose cylindrical coordinates, specify the axis using a rotation axis or two points.
For additional details on modeling momentum sources, see Momentum Sources in the CFX-Solver
Modeling Guide.
17.4.1.2. Equation Sources
Equation Sources introduces source terms to a particular scalar equation.
17.4.1.2.1. Component Mass Fractions
This will introduce a source of a particular component. A Source per unit volume or a Total Source
can be used. The optional Source Coefficient or Total Source Coefficient provides improved convergence for nonlinear sources. For details, see General Sources in the CFX-Solver Modeling Guide.
1.
In the Option and Source fields, set a component source term for a mixture.
This can be an expression or value for the total source or the source per unit volume. For details,
see General Sources in the CFX-Solver Modeling Guide.
2.
Set an optional Total Source / Source Coefficient.
For details, see Source Coefficient / Total Source Coefficient in the CFX-Solver Modeling Guide.
17.4.1.2.2. Additional Variables
A source for an Additional Variable can be set only if it is included in the parent domain and solved for
using a transport equation. (Poisson and Diffusive transports can also have sources.) A Source per unit
volume or a Total Source can be used. The optional Source Coefficient or Total Source Coefficient
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
183
Chapter 17: Subdomains
provides improved convergence for nonlinear sources. For details, see General Sources in the CFXSolver Modeling Guide.
1.
In the Option and Source fields, set an Additional Variable Source term.
For details, see General Sources in the CFX-Solver Modeling Guide.
2.
Set an optional Total Source / Source Coefficient.
For details, see Source Coefficient / Total Source Coefficient in the CFX-Solver Modeling Guide.
17.4.1.2.3. Continuity
Continuity sources differ from other sources because you are introducing new fluid into the domain.
Properties of the fluid entering the domain are required and appear in the Variables frame under the
Continuity section. For details on the following settings, see Mass (Continuity) Sources in the CFXSolver Modeling Guide.
•
Continuity > Source: Set a mass source value for the continuity equation.
•
Continuity > Option: Set the Fluid Mass Source per unit volume or the Total Fluid Mass
Source.
•
MCF/Energy Sink Option: Select the appropriate sink option from Local Mass Fractions and
Temperature, Specified Mass Fractions and Local Temperature, or Specified
Mass Fractions and Temperature, as appropriate.
•
Set a value for the Mass Flux Pressure Coefficient, Total Mass Source Pressure Coefficient or Mass
Source Pressure Coefficient, as appropriate.
•
Set a value for the Mass Flux Volume Fraction Coefficient, Total Mass Source Volume Fraction
Coefficient or Mass Source Volume Fraction Coefficient, as appropriate.
•
Set the variable values for the fluid that is introduced into the domain. The options available on this
section depend on the physical models used in the simulation. If the continuity source is negative, then
these parameters are not relevant except in the case when either Specified Mass Fractions
and Local Temperature, or Specified Mass Fractions and Temperature have been
selected for the MCF/Energy Sink Option.
–
Additional Variables: Set a value for each Additional Variables that is introduced with the mass
source.
–
Component Mass Fractions: Set the mass fraction for each of the components in the mass source.
–
Temperature: Enter the temperature for the mass source.
–
Set the mass source turbulence quantities as required by the selected turbulence model such as
Turbulence Eddy Dissipation and Turbulence Kinetic Energy.
–
Velocity: Set velocity components for the mass source.
17.4.1.2.4. Turbulence Quantities
When the flow is turbulent, sources can be specified for the required turbulence quantities such as
Turbulence Eddy Dissipation and Turbulence Kinetic Energy. A Source per unit
volume or a Total Source can be used. The optional Source Coefficient or Total Source Coefficient
provides improved convergence for nonlinear sources. For details, see General Sources in the CFXSolver Modeling Guide.
184
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh Motion
17.4.1.2.5. Energy
An Energy source can be specified when the parent domain models heat transfer using the Thermal
Energy or Total Energy model. A Source per unit volume or a Total Source can be used. The optional Source Coefficient or Total Source Coefficient provides improved convergence for nonlinear
sources. For details, see General Sources in the CFX-Solver Modeling Guide.
17.4.2. Bulk Sources for Multiphase Simulations
In a multiphase simulation, source terms that apply to all fluid in the simulation are set on the Sources
tab. Bulk sources take account of the volume fraction of each phase when applying the source term.
For details, see Bulk Sources in the CFX-Solver Modeling Guide.
1.
Select the Bulk Sources check box to specify bulk sources.
2.
Sources are set in the same way as for single phase simulations. For details, see Single-Phase Fluid
Sources (p. 182).
17.4.3. Multiplying Sources by Porosity
Selecting the Multiply by Porosity check box causes the equation source to be scaled by the porosity
value. For example, if a porous domain has a volume porosity of 0.8, then if the Multiply by Porosity
check box is selected, 80% of the source is applied to the fluid; if the check box is not selected then
100% of the source is applied to the fluid.
17.5. Fluids Tab
Fluid sources are used in an Eulerian multiphase simulation to apply volumetric source terms to individual fluids, and in particle transport to model absorption of particles in the subdomain. For details,
see Particle Absorption (p. 185).
1.
Select a fluid from the Fluid list to set fluid-specific sources.
2.
Toggle on the check box next to the fluid to expand the options.
3.
Sources are set in the same way as for single phase simulations. For details, see Single-Phase Fluid
Sources (p. 182).
It is important to note that these source terms are not automatically multiplied by the fluid volume
fraction (that is, do not automatically reduce to zero as the volume fraction goes to zero). For details,
see Fluid-Specific Sources in the CFX-Solver Modeling Guide.
17.5.1. Particle Absorption
This setting is available when particle tracking is modeled. For details, see Subdomains in the CFXSolver Modeling Guide.
1.
Select a particle type to activate particle absorption.
2.
Set the absorption diameter to the desired value.
17.6. Mesh Motion
When mesh deformation is selected for the domain that contains a subdomain, the Mesh Motion tab
is available for the subdomain.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
185
Chapter 17: Subdomains
The available options are:
•
Unspecified
•
Stationary
•
Specified Displacement
•
Specified Location
•
Rigid Body Solution
For details on these options, see Mesh Motion Options in the CFX-Solver Modeling Guide.
For details on mesh deformation, see Mesh Deformation in the CFX-Solver Modeling Guide.
See Mesh Deformation (p. 113) for information about activating mesh deformation for the domain.
186
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 18: Rigid Bodies
This chapter describes:
18.1. Rigid Body User Interface
A rigid body is a solid object that moves through a fluid without deforming. Its motion is dictated by
the fluid forces and torques acting upon it, plus any external forces (such as gravity) and external
torques. Within ANSYS CFX, a rigid body can be modeled in two ways:
•
A rigid body can be defined by a collection of 2D regions that form its faces. When a rigid body is
modeled in this way, the rigid body itself does not need to be meshed. Mesh motion is used to move
the mesh on the rigid body faces in accordance with the solution of the rigid body equations of motion.
•
Alternatively, an immersed solid can be defined as a rigid body. In this case the motion of the immersed
solid is dictated by the solution of the rigid body equations of motion.
Implementation information for Rigid Bodies is available in Rigid Body Theory in the CFX-Solver Theory
Guide.
18.1. Rigid Body User Interface
The user interface for setting up a rigid body defined as a collection of 2D regions is presented in the
following sections:
18.1.1. Insert Rigid Body Dialog Box
18.1.2. Basic Settings Tab
18.1.3. Dynamics Tab
18.1.4. Initial Conditions Tab
The user interface for setting up a rigid body implemented as an immersed solid consists of rigid body
settings found on the Basic Settings tab for the immersed solid domain. These settings are essentially
the same as those on the Basic Settings and Dynamics tabs in the details view for the rigid body object.
18.1.1. Insert Rigid Body Dialog Box
Use this method to simulate a rigid body by using a collection of 2D regions.
The Insert Rigid Body dialog box is used to initiate the creation of a new rigid body object. It is accessible
by clicking Rigid Body
, or by selecting Insert > Rigid Body.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
187
Chapter 18: Rigid Bodies
Note
Another way to simulate a rigid body is by using an immersed solid that uses a Domain
Motion option of Rigid Body Solution. In this case, the rigid body settings appear in
the details view for the immersed solid domain. All of the rigid body settings for an immersed
solid appear on the Basic Settings tab for the immersed solid domain. The analogous settings
for the rigid body object are distributed between the Basic Settings and Dynamics tabs of
the rigid body object. Although there are initialization settings on the Initialization tab of
the rigid body object, there are no corresponding initialization settings for a rigid body
defined as an immersed solid.
Immersed solids are described in Immersed Solids in the CFX-Solver Modeling Guide.
18.1.2. Basic Settings Tab
The Basic Settings tab for the rigid body object has the following settings:
18.1.2.1. Mass
Specify the mass of the rigid body. The mass is used in the calculation of translational acceleration due
to applied forces. It is also used in combination with the specified gravity vector (the gravity vector
specified with the rigid body, not with any buoyancy model) to calculate the force due to gravity. For
details, see Gravity (p. 191).
The force due to gravity acts through the specified center of mass. For details, see Center of Mass (p. 192).
18.1.2.2. Location
Specify all 2D regions (belonging to fluid domains) that physically contact the faces of the rigid body.
The forces and torques exerted by the fluid on all of these faces will contribute to the motion of the
rigid body. Note that if the rigid body is defined as an immersed solid, then the location is automatically
just the location of the immersed solid, and no further location setting is required.
To have these faces move automatically in accordance with the rigid body solution, you must also
specify that these faces have mesh motion provided by the rigid body solution. To do this, use the
Boundary Details tab in the details view for the boundary containing the faces. Additional faces or
mesh elements, which do not form part of the rigid body, can also have their mesh motion partially or
wholly specified by the rigid body solution. To do this, use the Boundary Details tab for boundaries
and the Mesh Motion tab for subdomains. Applying the rigid body solution to additional faces or mesh
elements could be used, for example, to help control the way the mesh distorts as the rigid body moves.
18.1.2.3. Coord Frame
You should specify a stationary coordinate frame that has its origin at the center of mass of the (physical) rigid body when the body is in its position at the start of the simulation. The coordinate frame you
specify must have the same orientation as the axes used to define the mass moment of inertia of the
body in its initial position (see Mass Moment of Inertia (p. 189)). In this documentation, this coordinate
frame is referred to as the rigid body coordinate frame. The position and orientation of the rigid body
are always calculated relative to this coordinate frame, and all other settings for the rigid body object
(for example, gravity and degrees of freedom) are with respect to this coordinate frame, unless otherwise
specified in this documentation.
188
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Rigid Body User Interface
If you choose a coordinate frame that does not have the position of the rigid body at the start of the
simulation, then you must specify an initial position for the rigid body (on the Initial Conditions tab)
that corresponds to the translation required to move the coordinate frame into the rigid body's initial
position. See Initial Conditions Tab (p. 191) for more information. Note that initial conditions settings are
not currently available for rigid bodies defined as immersed solids.
18.1.2.4. Mass Moment of Inertia
Specify absolute values of the components of the mass moment of inertia for the rigid body with respect
to a coordinate frame that:
•
Has the same initial orientation as the rigid body coordinate frame
•
Has its origin at the rigid body center of mass
•
Moves rigidly with the rigid body.
The mass moment of inertia components are used to define the mass moment of inertia matrix described
in Rotational Equations of Motion in the CFX-Solver Theory Guide.
For example, YY Component is defined as:
∫
− + − and XY Component is defined as:
∫
− − where the center of mass is given by
, and dm is a differential element of mass.
18.1.3. Dynamics Tab
The Dynamics tab for the rigid body object contains settings for the following items that influence the
motion of the rigid body:
•
External forces
•
External torques
•
Degrees of freedom of movement
•
Gravity vector.
With the exception of Rotational Degrees of Freedom all dynamics settings are in comparison to the
rigid body coordinate frame.
The Dynamics tab has the following settings:
18.1.3.1. External Force Definitions
External forces other than gravity are specified in the External Force Definitions frame. Use the Add
new item
list.
and Remove selected item
icons to add or remove external force definitions from the
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
189
Chapter 18: Rigid Bodies
Each external force definition has one of the following options:
•
None
This setting deactivates the external force.
•
Spring
These settings enable you to set up a spring force that is applied to the rigid body. Specify the
neutral position with respect to the rigid body coordinate frame via the Linear Spring Origin
settings. Whenever the center of mass of the rigid body is at the Linear Spring Origin, the applied
spring force is zero. The spring force develops as the center of mass of the rigid body moves away
from the neutral position, with a force-to-displacement ratio specified by the Linear Spring Constant. For details on how the center of mass is located, see Center of Mass (p. 192).
•
Value
These settings enable you to specify an external force using Cartesian force components (along
the principal axes of the rigid body coordinate frame).
The external forces are applied through the center of mass of the rigid body so that they cause translational accelerations only (and not any rotational accelerations).
18.1.3.2. External Torque Definitions
External torques are specified in the External Torque Definitions frame (in the details view). Use the
Add new item
the list.
and Remove selected item
icons to add or remove external torque definitions from
Each external torque definition has one of the following options:
•
None
This setting deactivates the external torque.
•
Spring
These settings enable you to set up a spring torque that is applied to the rigid body. Specify the
neutral orientation (with respect to the rigid body coordinate frame) via the Equilibrium Orientation
settings. You define the orientation using three angular displacements (specifically, Euler angles),
which are applied by the software using the ZYX convention:
–
The Euler Angle Z setting modifies the orientation by a rotation about the Z-axis (using the righthand rule to determine the direction).
–
The Euler Angle Y setting then further modifies the orientation by a rotation about the (modified)
Y-axis (using the right-hand rule to determine the direction).
–
The Euler Angle X setting then further modifies the orientation by a rotation about the (twice
modified) X-axis (using the right-hand rule to determine the direction).
These Euler angles are described in more detail in Rigid Body Motion in the CFX-Solver Modeling
Guide.
Whenever the orientation of the rigid body matches that specified by the Equilibrium Orientation
settings, the applied spring torque is zero. The spring torque develops as the rigid body rotates
190
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Rigid Body User Interface
away from the neutral orientation, with a torque-to-angular-displacement ratio specified by the
Torsional Spring Constant settings.
The torque develops due to changes in Euler angles, but is applied on the corresponding axes of
the rigid body coordinate frame. The torque spring implementation described here is recommended
for use only when both the equilibrium orientation and the rigid body orientation can be described
with small Euler angles (a few degrees).
•
Value
These settings enable you to specify an external torque using Cartesian torque components around
the principal axes of the rigid body coordinate frame.
18.1.3.3. Degrees of Freedom
18.1.3.3.1. Translational Degrees of Freedom
This setting determines the combination of axes along which the rigid body may translate. In this context,
the axes are those of the rigid body coordinate frame.
18.1.3.3.2. Rotational Degrees of Freedom
This setting determines the axes about which the rigid body may rotate. In this context, the axes are
of a coordinate frame that:
•
Has the same initial orientation as the rigid body coordinate frame
•
Has its origin at the rigid body center of mass
•
Moves rigidly with the rigid body.
18.1.3.4. Gravity
Specify a gravity vector in the rigid body coordinate frame that defines the downward direction and
the magnitude of free-fall acceleration due to gravity.
18.1.4. Initial Conditions Tab
The Initial Conditions tab contains settings for initializing the rigid body solver. These settings are
described in the following subsections.
Note
These settings are not available for rigid bodies defined as immersed solids.
Note
For the settings on the Initial Conditions tab, the Automatic option provides initial values
of zero, and the Automatic with Value option provides initial values as specified. In both
cases, the values used at the beginning of a restarted run are taken from the results of the
previous run. When you restart a run, select Continue History From and choose initial values
from the previous results. To access this option, you should be in the Define Run dialog box
of CFX-Solver Manager and both Initial Values Specification and Continue History From
must be selected.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
191
Chapter 18: Rigid Bodies
18.1.4.1. Center of Mass
These settings define the location (in the rigid body coordinate frame) of the center of mass of the rigid
body at the start of the simulation. These settings should be set with non-zero values only if the origin
of the rigid body coordinate frame is not at the center of mass of the rigid body at the start of the
simulation. If non-zero values are required, then they represent the translation from the origin of the
rigid body coordinate frame to the position of the rigid body center of mass at the start of the simulation.
Note
Setting non-zero values for the Center of Mass settings does not impose a mesh motion at
the start of the simulation; rather, the initial position of the mesh is assumed to represent
the physical location of the rigid body at the start of the simulation.
Note
It is recommended that you define a rigid body coordinate frame that has its origin located
at the initial center of mass of the rigid body (that is, the center of mass of the rigid body
as positioned in the initial mesh). You could then set all the Center of Mass settings on the
Initial Conditions tab to zero (or select the Automatic option to set the initial values to
zero automatically).
18.1.4.2. Linear Velocity
These settings initialize the translational velocity of the rigid body in the rigid body coordinate frame.
The velocity components are taken as being along the principal axes of the rigid body coordinate frame.
18.1.4.3. Angular Velocity
These settings initialize the angular velocity of the rigid body in the rigid body coordinate frame. The
angular velocity components are taken as being about the principal axes of the rigid body coordinate
frame, using the right-hand rule to establish direction.
18.1.4.4. Linear Acceleration
These settings initialize the translational acceleration of the rigid body in the rigid body coordinate
frame. The acceleration components are taken as being along the principal axes of the rigid body coordinate frame.
18.1.4.5. Angular Acceleration
These settings initialize the angular acceleration of the rigid body in the rigid body coordinate frame.
The angular acceleration components are taken as being about the principal axes of the rigid body
coordinate frame, using the right-hand rule to establish direction.
192
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 19: Units and Dimensions
This chapter describes:
19.1. Units Syntax
19.2. Using Units in CFX-Pre
19.3. Setting the Solution Units
19.1. Units Syntax
Dimensional quantities are defined in units or a combination of units. For example, mass can have units
of [kg], [g] or [lb] (and many others); pressure can have units of [atm], [N m^-2] and [Pa] (and many
others).
The general units syntax in CFX is defined as [multiplier|unit|^power] where multiplier is a multiplying
quantity (such as mega, pico, centi, and so on), unit is the unit string (kg, m, J, and so on), and power
is the power to which the unit is raised. When typing units in expression, they must be enclosed by
square brackets, [...]. You will usually not see the brackets when selecting units from a list of commonly
used units. In general, units declarations must obey the following rules:
•
A units string consists of one or more units quantities, each with an optional multiplier and optional
power. Each separate units quantity is separated by one or more spaces.
•
Short forms of the multiplier are usually used. n stands for nano, µ stands for micro, c for centi, k for
kilo, m for milli, M for mega and G for giga.
•
Powers are denoted by the ^ (caret) symbol. A power of 1 is assumed if no power is given.
Note
The / operator is not supported, so a negative power is used for unit division (for example, [kg m^-3] corresponds to kilograms per cubic meter).
•
If you enter units that are inconsistent with the physical quantity being described, then a dialog box
will appear informing you of the error, and the units will revert to the previous units.
•
Units do not have to be given in terms of the fundamental units (mass, length, time, temperature, angle
and solid angle). For instance, Pa (Pascals) and J (Joules) are both acceptable as parts of unit strings.
•
Units strings are case sensitive; for example, Kg and KG are both invalid parts of units strings.
To give the units of dynamic viscosity, which has the dimensions of Mass Length-1 Time-1, the unit
string [kg m^-1 s^-1] (or [lb ft^-1 hr^-1]) is valid.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
193
Chapter 19: Units and Dimensions
Note
The following unit strings are invalid:
[kg/(metre sec)]
[kg/(ms)]
[kg/m/s]
[kg/(m.s)]
[kg/(m s)]
[kg/(m*s)]
[kg/(m sec)]
[lb/(ft hr)]
19.2. Using Units in CFX-Pre
There are a number of Details views in CFX-Pre that require the entry of physical quantities. For example,
when you set the physical properties for a fluid, or enter values for boundary conditions, the units in
which you input the data must be selected.
A list of possible units for the quantity of interest is provided, but you may want to use an expression
for the quantity, in which case you must specify the units. You can use any units that are consistent
with the quantity you are describing. The default units in CFX-Pre are SI.
The units selector is automatically filled in using the default units for the quantity. You can select other
commonly used units for that quantity from the drop-down list in the units selector.
19.2.1. Units Commonly Used in CFX
CFX-Pre provides you with a choice of several commonly used units to ease the task of specifying
quantities and converting results.
The full list of quantities where commonly used units are available is given in the following table:
Quantity
Commonly used units
Velocity
[m s^-1]
[km hr^-1]
[mile hr^-1]
[ft s^-1, knot]
Volumetric Flow
[m^3 s^-1]
[litre s^-1]
[gallon hr^-1]
[gallonUSliquid hr^-1]
Mass Flow
[kg s^-1]
[tonne s^-1]
[lb s^-1]
194
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Using Units in CFX-Pre
Quantity
Commonly used units
k (turbulence kinetic energy)
[m^2 s^-2]
[J kg^-1]
Epsilon (turbulence dissipation rate)
[m^2 s^-3]
Pressure
[Pa]
[J kg^-1 s^-1]
[N m^-2]
[bar]
[torr]
[mm Hg]
[psi]
[psf ]
Concentration
[m^-3]
[litre^-1]
[foot^-3]
Dynamic Viscosity
[kg m^-1 s^-1]
[centipoise]
[g cm^-1 s^-1]
[N s m^-2]
[Pa s]
[dyne s cm^-2]
[lb ft^-1 hr^-1]
[lbf s ft^-2]
Thermal Conductivity
[W m^-1 K^-1]
[cal cm^-1 s^-1 K^-1]
[BTU (ft^2 s (F/ft))^-1]
[BTU (ft^2 hr (F/ft))^-1]
Specific Heat Capacity
[J kg^-1 K^-1]
[cal g^-1 K^-1]
[J g^-1 K^-1]
[BTU lb^-1 F^-1]
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
195
Chapter 19: Units and Dimensions
Quantity
Commonly used units
Thermal Expansivity
[K^-1]
Kinematic Diffusivity
[m^2 s^-1]
[cm^2 s^-1]
Acceleration
[m s^-2]
[ft s^-2]
Temperature
[K]
[C]
[R]
[F]
Density
[kg m^-3]
[g cm^-3]
[lb ft^-3]
Mass Concentration
[kg m^-3]
[g l^-1]
Mass Fraction
[kg kg^-1]
[g kg^-1]
Length
[m]
[mm]
[foot]
[in]
Mass Flow in
[kg s^-1]
[tonne s^-1]
[lb s^-1]
Volumetric Flow in
[m^3 s^-1]
[litre s^-1]
[gallon hr^-1]
[gallonUSliquid hr^-1]
Heat Transfer Coefficient
[W m^-2 K^-1]
Heat Flux in
[W m^-2]
Time
[s]
[min]
196
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Setting the Solution Units
Quantity
Commonly used units
[hr]
Shear Strain rate
[s^-1]
Energy Source
[W m^-3]
[kg m^-1 s^-3]
Energy Source Coefficient
[W m-^3 K^-1]
[kg m^-1 s^-3 K^-1]
Momentum Source
[kg m^-2 s^-2]
Momentum Source Lin. Coeff.
[kg m^-3 s]
Momentum Source Quad.
Coeff.
[kg m^-4]
Per Time
[s^-1]
Angle
[radian]
[degree]
Angular Velocity
[radian s^-1]
[rev min^-1]
Specific Enthalpy
[J kg^-1]
[m^2 s^-2]
Energy
[J]
19.2.2. Defining Your Own Units
The commonly used units array is only a subset of the possible units you can use in CFX-Pre. Each unit
is a combination of one or more base dimensions. To specify your own units for a quantity, click the
Enter Expression icon
for the associated variable and type the value and units into the data area
using the syntax. For details, see Units Syntax (p. 193).
There are many base units to choose from; most units in common use are valid as parts of unit strings.
You can specify any quantity in any valid units as long as you adhere to the units definition syntax.
19.3. Setting the Solution Units
There are two sets of units in CFX-Pre: the units visible when selecting Edit > Options from the main
menu, which are also used for mesh import and transformation, and the solution units set in the Solution
Units details view (available from the main menu under Insert > Solver). The solution units are the
units that the CFX-Solver writes in the results file. For details, see Units (p. 48).
Setting the solution units does not alter the units you can use to define quantities in CFX-Pre. These
are the units the results file is written in. Additionally, these are the units assumed in the summary at
the end of the out file, when data such as variable range and forces on walls is presented.
When post-processing a results file in CFD-Post, the units used are not necessarily those used in the
results file. CFD-Post will convert to your preferred units.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
197
Chapter 19: Units and Dimensions
Most common units can be used for the solution units; however, some important restrictions apply:
•
The temperature solution units must be an absolute scale; for example, Kelvin [K] or Rankine [R]. Celsius
and Fahrenheit cannot be used. Temperature quantities elsewhere in CFX-Pre can be set in Celsius and
Fahrenheit.
•
The solution units must not be changed when restarting a run. The units in the initial guess file will
assume the units used in the current CFX-Solver definition (.def) file.
•
You must not change the length units outside of CFX-Pre, for example, by editing the CCL in a CFXSolver input file. The mesh is written to the CFX-Solver input file using the length units; therefore, once
the CFX-Solver input file has been written, these units should not change.
198
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 20: Solver Control
Solver Control is used to set parameters that control the CFX-Solver during the solution stage.
This chapter describes:
20.1. Basic Settings Tab
20.2. Equation Class Settings Tab
20.3. External Coupling Tab
20.4. Particle Control Tab
20.5. Rigid Body Control Tab
20.6. Advanced Options Tab
You can find further help on setting solver parameters in Advice on Flow Modeling in the CFX-Solver
Modeling Guide.
20.1. Basic Settings Tab
The Basic Settings tab controls following common and simulation specific parameters:
•
Basic Settings: Common (p. 199)
•
Basic Settings for Steady State Simulations (p. 201)
•
Basic Settings for Transient Simulations (p. 201)
•
Immersed Solid Control (p. 202)
20.1.1. Basic Settings: Common
20.1.1.1. Advection Scheme
For details, see Advection Scheme Selection in the CFX-Solver Modeling Guide.
20.1.1.2. Turbulence Numerics
The Turbulence Numerics options are First Order and High Resolution. The First Order
option uses Upwind advection and the First Order Backward Euler transient scheme. The
High Resolution option uses High Resolution advection and the High Resolution transient
scheme.
For details, see Advection Scheme Selection in the CFX-Solver Modeling Guide and Transient Scheme in
the CFX-Solver Modeling Guide.
Note
The Turbulence Numerics settings will override the settings on the Equation Class Settings
Tab (p. 203).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
199
Chapter 20: Solver Control
20.1.1.3. Convergence Criteria
For details, see Monitoring and Obtaining Convergence in the CFX-Solver Modeling Guide.
•
Residual Type: select either RMS or MAX.
•
Residual Target: specify a value for the convergence.
For details, see Residual Type and Target in the CFX-Solver Modeling Guide.
•
Conservation Target: optionally specify the fractional imbalance value. The default value is 0.01.
For details, see Conservation Target in the CFX-Solver Modeling Guide.
20.1.1.4. Elapsed Wall Clock Time Control
Select the Maximum Run Time option if you want to stop your run after a maximum elapsed time
(wall clock time).
If you select this option the flow solver will automatically attempt to estimate the time to complete the
next timestep or outer loop iteration. The estimated time is the average time that it takes to solve a
previous iteration (includes the time to assemble and solve the linear equations, radiation and particle
tracking) plus the average time it is taking to write any Standard backup or transient files. The time
estimate currently does not include the time used by processes external to the flow solver. This includes
mesh refinement, interpolation and FSI with Mechanical.
20.1.1.5. Interrupt Control
Interrupt control conditions are used to specify the interrupt criteria for a solver run. These conditions
are specified using logical expressions that are evaluated by CFX-Solver and reported in the CFX output
file. After executing each coefficient iteration and time step (or outer iteration), the solver evaluates all
internal termination conditions and user defined interrupt control conditions. If any of these conditions
are true, then solver execution stops and the outcome is written to the CFX output file.
Typically, interrupt control conditions are defined by single-valued logical expressions. However, singlevalued mathematical expressions can also be used. In this case, a single-valued mathematical expression
is considered to be true if, and only if, the result of the expression is greater than or equal to 0.5. Otherwise it is deemed to have a value of false. For a discussion of logical expressions, see CFX Expression
Language Statements in the CFX Reference Guide.
20.1.1.5.1. List Box
The list box is used to select interrupt control conditions for editing or deletion. Interrupt control conditions can be created or deleted with icons that appear beside the list box.
20.1.1.5.1.1. [Interrupt Condition Name]
Enter a logical expression to specify an interrupt control condition.
20.1.1.6. Junction Box Routine
If you have created any Junction Box Routine objects, select those to include in this Solver run.
For details, see User Junction Box Routines in the CFX-Solver Modeling Guide.
200
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Basic Settings Tab
20.1.2. Basic Settings for Steady State Simulations
20.1.2.1. Convergence Control: Min. Iterations
The minimum number of iterations the CFX-Solver will run.
20.1.2.2. Convergence Control: Max. Iterations
The maximum number of iterations the CFX-Solver will run.
For details, see Max. Iterations in the CFX-Solver Modeling Guide.
20.1.2.3. Convergence Control: Fluid Timescale Control
Sets the method of time scale control for a simulation. For details, see Time Scale Control in the CFXSolver Modeling Guide.
Three options are available for steady state simulations:
•
Auto Timescale: For details, see Auto Timescale in the CFX-Solver Modeling Guide and Automatic
Time Scale Calculation in the CFX-Solver Theory Guide.
–
Length Scale Option
Three options are available: Conservative, Aggressive or Specified Length Scale.
•
Local Timescale Factor: For details, see Local Time Scale Factor in the CFX-Solver Modeling Guide.
•
Physical Timescale: For details, see Physical Time Scale in the CFX-Solver Modeling Guide.
20.1.2.4. Solid Timescale Control
This option is available in a steady state simulation when a solid domain, or a solid within a porous
domain, is used. Two choices are available: Auto Timescale and Physical Timescale.
•
Solid Timescale Factor: This option is available when Auto Timescale is used as the Solid Timescale.
For details, see Solid Time Scale Control in the CFX-Solver Modeling Guide.
20.1.3. Basic Settings for Transient Simulations
20.1.3.1. Transient Scheme
For details, see Transient Scheme in the CFX-Solver Modeling Guide.
20.1.3.2. Convergence Control
You will have already specified the number of timesteps under Analysis Type. For details, see Analysis
Type (p. 101).
20.1.3.2.1. Min. Coeff. Loops
This option determines the minimum number of iterations per timestep, and has a default value of 1.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
201
Chapter 20: Solver Control
Important
If a compressible transient flow is undertaken with only one iteration per time step, then the
solution can be incorrect if the Heat Transfer option is not set to Total Energy, or if heat
transfer is not included in the simulation. This is due to the CFX-Solver not extrapolating the
pressure at the start of the time step in these circumstances. This means that density is not
extrapolated, and so the solver cannot calculate an accurate value for the time derivative of
density on the first iteration. The workaround for this problem is to either run with at least
two iterations per time step, or to use the Total Energy option for Heat Transfer.
20.1.3.2.2. Max. Coeff. Loops
This option determines the maximum number of iterations per timestep, and has a default value of 10.
For details, see Max. Iter. Per Step in the CFX-Solver Modeling Guide.
20.1.3.2.3. Fluid Timescale Control
Coefficient Loops is the only available option.
20.1.4. Immersed Solid Control
The immersed solid is represented as a source term in the fluid equations that drives the fluid velocity
to match the solid velocity. The size of the source term is controlled by the Momentum Source Scaling
Factor setting, which can be set globally (in the global Solver Control settings) or for individual immersed solids (on the immersed solid domain Solver Control tab). The default value of 10 is acceptable
most of the time. If robustness problems are encountered, the scaling factor may be decreased (for
example by a factor of 2), but at the expense of accuracy; the difference between the fluid velocity and
the specified solid velocity will generally increase, even if only by a small amount.
Boundary Model has two options:
•
None
This is the default option.
•
Modified Forcing
This option enables modifications to the immersed solid source term to take better account of the
boundaries of the immersed solid and their effect on the flow.
If you set Boundary Model to Modified Forcing, then the Boundary Tracking setting is available.
The Boundary Tracking setting has two options:
•
Boundary Face Extrusion
Once Boundary Model is selected, this is the default option.
The Boundary Face Extrusion option requires you to specify two settings that must be set
appropriately so that each near-wall node can be reliably projected onto the best location on the
immersed boundary face. These settings are:
–
202
Extrusion Distance
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Equation Class Settings Tab
This is the distance by which each immersed boundary face is extruded outward from, and
normal to, the immersed boundary to form an imaginary volume. A bounding box, that consists
of faces of constant x, y, and z coordinate, is then constructed around each imaginary volume.
If a near-wall node falls within the bounding box, then CFX-Solver will project that near-wall
node normal to and onto the plane of the boundary face. If the projected location lies outside
the face, other mechanisms take effect to find the nearest suitable projected location.
The value of Extrusion Distance should be of the order of magnitude of the length of a fluid
mesh element in the vicinity of the immersed boundary.
–
Extrusion Tolerance
This is a factor by which the solver will multiply the edge length of the bounding box for each
imaginary volume. The bounding box is mentioned in the description for the Extrusion Distance
setting. An overly large value will cause near-wall nodes to be mapped to locations on boundary
faces that are not necessarily the closest face.
The default value for Extrusion Tolerance is 0.01.
•
Search Through Elements
When using this option, CFX-Solver will search through elements near the immersed boundary and
project the near-immersed-boundary fluid nodes onto the face edge or vertices of the immersed
solid element. This option requires no user input.
This method is less accurate than the Boundary Face Extrusion option, but can be used for
cases where no suitable Extrusion Distance can be determined.
For details see Immersed Boundary Tracking in the CFX-Solver Modeling Guide.
20.2. Equation Class Settings Tab
Equation class settings allow you to control some aspects of the CFX-Solver on an equation class basis.
For example, you can set a different time scale or advection scheme as well as convergence control
and criteria parameters for each class of equations. This is useful if you suspect a convergence problem
is caused by a particular equation class; you can then use a smaller timestep or a more robust advection
scheme for that equation class.
•
Select the equation class for which to specify settings.
•
The settings in this tab are a subset of those found on the Basic Settings tab (see Basic Settings: Common (p. 199)).
For details, see Timestep Selection in the CFX-Solver Modeling Guide and Advection Scheme Selection
in the CFX-Solver Modeling Guide.
The settings you specify on this form will override those on the Basic Settings tab. Any equation classes
that are unspecified will use the parameters set on the Basic Settings tab. The number and type of
equation classes depends on the specific physics of the problem.
For a free surface simulation, you cannot set the advection scheme for the volume fraction (vf ) equation
class because the CFX-Solver uses a special compressive advection scheme.
For details, see Controlling the Timescale for Each Equation in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
203
Chapter 20: Solver Control
20.3. External Coupling Tab
This section is visible when External Solver Coupling is set to ANSYS MultiField on the Analysis
Type tab.
For details, see Solver Controls, External Coupling Tab in the CFX-Solver Modeling Guide.
20.4. Particle Control Tab
This section is visible when particle tracking has been selected. For details, see Particle Solver Control
in the CFX-Solver Modeling Guide.
20.5. Rigid Body Control Tab
The following options handle control of the rigid body solver.
The Update Frequency setting controls when the rigid body solver updates the position of the rigid
body. The options are:
•
Every Iteration (steady-state simulations only)
This option causes the rigid body solver to update the position of the rigid body at the beginning of each iteration.
•
Every Time Step (transient simulations only)
This option causes the rigid body solver to update the position of the rigid body at the beginning of each time step.
This option is recommended only for weakly-coupled systems (for example, where fluid flow
changes within a single time step have little effect on the rigid body motion) or when the
time step is very small.
•
Every Coefficient Loop (transient simulations only)
This option:
•
–
Causes the rigid body solver to update the position of the rigid body at the beginning of each
coefficient loop within each time step.
–
Is recommended when there is tight coupling between the fluid flow and the motion of the
rigid body.
–
Is more computationally expensive than the Every Time Step option
–
Can cause issues if the flow solver requires several coefficient loop iterations to stabilize the
applied forces/torques between calls to the rigid body solver.
General Coupling Control
This option causes the rigid body solver to update the position of the rigid body during each
"stagger" (or coupling) iteration.
During every stagger iteration, the following sequence occurs:
1.
204
The rigid body solver reads the latest calculated forces and torques.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Rigid Body Control Tab
2.
The rigid body solver solves to determine the new rigid body state (position, orientation, velocity, and so on).
3.
The CFX flow solver reads the new rigid body state.
4.
The CFX flow solver solves all the field equations, including mesh motion where appropriate,
by performing outer loop iterations (steady-state cases) or coefficient loop iterations (transient
cases) until either the maximum number of iterations/coefficient loops is reached, or until all
the field equations have converged. The mesh motion solution uses the latest rigid body state
in order to calculate the mesh motion on all boundaries or subdomains set to use the rigid
body solution. If the rigid body is an immersed solid, then the latest rigid body state is used
to calculate the motion of the immersed solid domain.
Stagger iterations are repeated until the maximum number of stagger iterations is reached or
until the time step (transients runs) or simulation (steady-state runs) is deemed to have converged, when the following criteria are met:
–
The rigid body solver has converged (angular equations only),
–
The force, torque and mesh motion data transferred between the CFX flow solver and the rigid
body solver satisfy the appropriate convergence criteria, AND
–
All the CFX field equations (mesh motion, mass and momentum, energy, and so on) have converged to the appropriate convergence criteria.
When the time step (transient runs) is converged, then this guarantees an implicit solution of
all solution fields for each time step, providing the most stability when there is a strong
coupling between the fluid flow and the motion of the rigid body.
The Internal Coupling Step Control settings set limits on the minimum and maximum
number of stagger iterations.
When the Every Iteration, Every Coefficient Loop, or General Coupling Control
option is selected, the Internal Coupling Data Transfer Control settings are available. These settings
include:
•
Mesh Motion Data Transfer Control
•
Force Data Transfer Control
•
Torque Data Transfer Control
For each of these Internal Coupling Data Transfer Control settings, you may:
•
Optionally specify an Under Relaxation Factor for aiding convergence. The default value is 0.75 for all
three transferred quantities. If a case has difficulty converging due to overshoots in the force, torque
and/or mesh motion quantities passed between the two solvers, then the under-relaxation factor for
one or more quantities can be reduced to damp down the overshoots. Values that are too small will
tend to increase the number of iterations needed for convergence. On the other hand, for a case where
the force, torque and mesh motion are steady and don't change much from time step to time step, it
may be possible to raise the under-relaxation factors to 1 to speed up convergence.
•
Optionally specify a Convergence Target.
The convergence target is the target value of the convergence measures described below.
–
For Mesh Motion Data Transfer Control, the convergence measure is the maximum of:
→ The distance from the previous to the current center of mass, divided by the greater of the previous and current distances from the center of mass to the rigid body coordinate frame origin.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
205
Chapter 20: Solver Control
Here, “previous” refers to the previous stagger iteration, coefficient loop, and so on — whenever
the rigid body solver was last called.
→
+
+
+
−
− 
, where =  
−
, n refers to the current

iteration (stagger iteration, coefficient loop, and so on — whenever the rigid body solver was
last called), − refers to the previous iteration, and =   is the orientation


quaternion, with q0 being the scalar component and q1, q2, q3 being the vector components.
Here, all quantities are with respect to the rigid body coordinate frame.
–
For Force Data Transfer Control, the convergence measure is:
The magnitude of the change (from the previous value to the current value) in net force divided
by the greater of the previous magnitude of the net force and the current magnitude of the
net force, where “previous” refers to the previous stagger iteration, coefficient loop, and so on
— whenever the rigid body solver was last called.
–
For Torque Data Transfer Control, the convergence measure is:
The magnitude of the change (from the previous value to the current value) in net torque divided
by the greater of the previous magnitude of the net torque and the current magnitude of the
net torque, where “previous” refers to the previous stagger iteration, coefficient loop, and so
on — whenever the rigid body solver was last called.
The convergence measures are plotted on the Rigid Body Convergence tab in CFX-Solver Manager
when running a simulation that involves the rigid body solver. For details on the plots available
for such runs, see Monitor Plots related to Rigid Bodies in the CFX-Solver Modeling Guide.
The Angular Momentum Equation Control settings are:
•
Integration Method
An iterative process is used to calculate the solution to the angular momentum equation.
Choose one of the following options to control the integration method for this process:
–
First Order Backward Euler
This option provides first-order accuracy, and is vulnerable to gimbal lock problems. For
details, see First Order Backward Euler in the CFX-Solver Theory Guide.
–
Simo Wong
This option provides second-order accuracy For details, see Simo Wong Algorithm in the
CFX-Solver Theory Guide.
The Iteration Convergence Criterion > Iteration Convergence setting controls the degree
to which an orientation must remain the same between successive iterations in order for
the solution to be considered converged. The value is a normalized quantity; the default
should be sufficient for most purposes.
The Maximum Number of Iterations > Max. Iterations setting (which controls the maximum number of iterations used by the Simo Wong integration method) can be increased
if you see any warnings in the solver output that indicate a lack of convergence for the
integration method.
206
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Advanced Options Tab
20.6. Advanced Options Tab
The parameters on the Advanced Options tab should not need to be changed for most simulations.
Dynamic Model Control
When Global Dynamic Model Control is selected, it enables some special modes to be implemented
in the solver for the first few iterations or timesteps. For details, see Advanced Options: Dynamic Model
Control in the CFX-Solver Modeling Guide.
For details on Turbulence Control, see Turbulence Control in the CFX-Solver Modeling Guide.
For details on Combustion Control, see Advanced Combustion Controls in the CFX-Solver Modeling
Guide.
For details on Hydro Control, see Hydro Control in the CFX-Solver Modeling Guide.
Pressure Level Information
Sets an X/Y/Z location for reference pressure and a pressure level.
For details, see Pressure Level Information in the CFX-Solver Modeling Guide.
Thermal Radiation Control
For details, see Thermal Radiation Control in the CFX-Solver Modeling Guide.
Body Forces
Under this option, Volume-Weighted should be generally used except for free surface cases.
For details, see Body Forces in the CFX-Solver Modeling Guide.
Interpolation Scheme
For details, see Interpolation Scheme in the CFX-Solver Modeling Guide.
Multicomponent Energy Diffusion
This option is available when a multicomponent flow is used with a heat transfer equation (that is,
thermal or total energy). For details, see Multicomponent Energy Diffusion in the CFX-Solver Modeling
Guide. The possible options are:
•
Automatic: uses unity Lewis number when no component diffusivities specified and no algebraic slip
model; uses generic assembly when necessary
•
Generic Assembly: sets default component diffusivities to unity Schmidt number Sc = 1; generic
treatment of energy diffusion term with support for user defined component diffusivities and algebraic
slip model
•
Unity Lewis Number: sets Le = 1; single diffusion term, rather than separate term for contribution
of every component, resulting in faster solver runs; the default molecular diffusion coefficient for components is derived from thermal conductivity
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
207
Chapter 20: Solver Control
Note
Forcing unity Lewis number mode when not physically valid may lead to inconsistent
energy transport. Therefore this setting is not recommended.
Temperature Damping
For details, see Temperature Damping in the CFX-Solver Modeling Guide.
Velocity Pressure Coupling
The Rhie Chow Option controls the details of the Rhie Chow pressure dissipation algorithm. Fourth
Order ensures that the dissipation term vanishes rapidly under mesh refinement. However, it can
sometimes induce wiggles in the pressure and velocity fields; for example, near shocks. The Second
Order option damps out these wiggles more rapidly, but is also less accurate. The High Resolution
option uses Fourth Order as much as possible, but blends to Second Order near pressure extrema. It is
a good choice for high speed flow. The default is Fourth Order for most simulations, but High
Resolution is automatically chosen if High Speed Numerics is activated under Compressibility
Control on the Solver Control tab. The High Resolution option may occasionally be useful in
other situations as well. For example, if you observe the simulation diverging and continuity residuals
are significantly higher than the momentum residuals prior to divergence.
Compressibility Control
The following options control parameters that affect solver convergence for compressible flows.
The Total Pressure Option controls the algorithm used for static-to-total conversions (and vice versa).
There are three possible settings:
Incompressible
The incompressible assumption is used in all situations.
Automatic
The total pressure is calculated depending on the equation of state.
Unset
This is equivalent to Automatic when the total energy model is used, and Incompressible otherwise.
For further details, see Total Pressure in the CFX-Solver Theory Guide.
The Automatic option may experience robustness problems for slightly compressible fluids (such as
compressible liquids). In such cases, you should consider using the Incompressible option instead.
When the High Speed Numerics option is selected, special numerics are activated to improve solver
behavior for high-speed flow, such as flow with shocks. This setting causes three types of behavior
changes. Firstly, it activates a special type of dissipation at shocks to avoid a transverse shock instability
called the carbuncle effect (which may occur if the mesh is finer in the transverse direction than in the
flow direction). Secondly, it activates the High Resolution Rhie Chow option to reduce pressure wiggles
adjacent to shocks. Finally, for steady state flows, it modifies the default relaxation factors for the advection blend factor and gradients.
The Clip Pressure for Properties option enables the solver to accept negative absolute pressures in
the converged solution. For simulations involving compressible flow, the absolute pressure should not
208
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Advanced Options Tab
be negative. However, the pressure field required to satisfy the governing equations on a finite mesh
may not necessarily satisfy this condition. By default, the solver is robust to a pressure field that may
want to temporarily lead to negative pressures, but not if negative pressures are present in the converged
solution. The solver can be made robust to negative absolute pressures in the converged solution by
activating this parameter, which clips the absolute pressure to a finite value when evaluating pressuredependent properties such as density.
Multiphase Control
The following options handle control of solver details specific to multiphase flows.
When the Volume Fraction Coupling option is set to Segregated, the solver solves equations for
velocity and pressure in a coupled manner, followed by solution of the phasic continuity equations for
the volume fractions. With the Coupled option, the solver implicitly couples the equations for velocity,
pressure, and volume fraction in the same matrix. The coupled algorithm is particularly beneficial for
buoyancy-dominated flows, such as buoyant free surface problems.
The Initial Volume Fraction Smoothing option can be set to None or Volume-Weighted. If the
initial conditions for volume fraction have a discontinuity, startup robustness problems may occur.
Choosing Volume-Weighted smoothing of these volume fractions may improve startup robustness.
Intersection Control
You can use the options described in this section to control the intersection of non-matching meshes.
The parameters that you set here are applied to all interfaces where Intersection Control settings have
not been applied individually in domain interface definitions. (See Intersection Control (p. 145) to learn
how to apply Intersection Control settings to individual interfaces.)
CFX provides the GGI (General Grid Interface) capability, which determines the connectivity between
the meshes on either side of the interface using an intersection algorithm. In general, two intersection
methods are provided:
•
Bitmap Intersection:
Two faces on either side of the interface which have to be intersected are both drawn into an
equidistant 2D pixel map. The area fractions are determined by counting the number of pixels that
reside inside both intersected faces (that is, within the union of the two faces). The area fraction
for a face is then calculated by dividing the number of overlapping pixels by the total number of
pixels in the face. This method is very robust.
•
Direct Intersection (Default):
Two faces on either side of the interface are intersected using the Sutherland-Hodgeman clipping
algorithm. This method computes the exact area fractions using polygon intersection, and is much
faster and more accurate than the bitmap method.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
209
Chapter 20: Solver Control
Note
•
If Direct (one-to-one) mesh connectivity is available, the solver will ignore the Intersection
Control option and will instead use a 'topological intersection', that is, use the one-to-one
information to generate the intersection data.
•
If you are restarting a run, the intersection step is skipped and the intersection data is read
from the results file. This behavior can be overridden by setting the expert parameter force
intersection to True.
The Bitmap Resolution controls the number of pixels used to fill the 2D pixel map (see description of
the bitmap intersection method above). The higher this number, the more accurate the final calculation
of the area fractions. In general, the default resolution of 100 should be sufficient but large differences
in the mesh resolution on both sides of the interface as well as other mesh anomalies may require the
bitmap resolution to be increased. Larger numbers will cause longer intersection times, for example,
doubling the bitmap resolution will approximately quadruple the GGI intersection time.
When the Permit No Intersection option is set, the solver will run when there is no overlap between
the two sides of an interface. This parameter is mainly useful for transient cases where interface geometry
is closing and opening during the run. For example, transient rotor-stator cases with rotating valves, or
moving mesh cases where the GGI interface changes from overlap to non-overlap during the simulation
both can exhibit this type of behavior. This parameter is not switched on by default.
The Discernible Fraction option controls the minimum area fraction below which partially intersected
faces are discarded. The following default values used by the solver depend on the intersection method:
•
Bitmap Intersection: 1/(Bitmap Resolution)^1.5
•
Direct Intersection: 1.0E-06
The idea is that intersection inaccuracies should not lead to tiny area fractions that have no impact on
the solution.
The Edge Scale Factor option is used to control the detection of degenerate faces. Degenerate faces
are detected by comparing the face edge lengths with a characteristic length of the volume touching
the face. Degenerated faces will not be intersected and therefore, intersected faces of zero size are
discarded so that problems with the 2D projection of those faces are avoided.
The Periodic Axial Radial Tolerance option is used when determining if the surface represented by
the interface is a constant axial or radial surface. For a rotational periodic GGI interface, the solver ensures
that the ratio of the radial and axial extent compared to the overall extent of each interface side is
bigger than the specified value and therefore, the interface vertices do not have the same radial or
axial positions.
The Circumferential Normalized Coordinates Option is used to set the type of normalization applied
to the axial or radial position coordinates (η). Mesh coordinate positions on GGI interfaces using pitch
change are transformed into a circumferential (θ) and axial or radial position (η). The η coordinates span
from hub to shroud and are normalized to values between 0 and 1. In cases where the hub and/or
shroud curves do not match on side 1 and side 2, different approaches are available to calculate the
normalized η coordinates based on side local or global minimum and maximum η values:
•
210
Mixed (Default for Fluid Fluid interfaces): Normalization of η is based on local minimum and maximum
η values as well as the η range of side 1. This method forces the hub curves on side 1 and 2 to align.
Non-overlap regions adjacent to the shroud may be produced if the shroud curves are not the same.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Advanced Options Tab
•
Global (Default for Fluid Solid Interfaces): Normalization of η is based on global minimum and maximum
eta values. This method intersects side 1 and 2 unchanged from their relative positions in physical coordinates. If the hub and shroud curves do not match then non-overlap regions will be produced.
•
Local: Normalization of η is done locally for each side of the interface. This method will always produce
an intersection of side 1 and 2, but may cause undesirable scaling of the geometry in some cases.
The Face Search Tolerance Factor is a scaling factor applied to the element sized based separation
distance used to find candidates for intersection. For a given face on side 1 of the interface, candidate
faces for intersection are identified on side 2 using an octree search algorithm. The octree search uses
this tolerance to increase the sizes of the bounding boxes used to identify candidates. Making this
parameter larger will increase the size of the bounding boxes, resulting in possible identification of
more candidates.
The Face Intersection Depth Factor is a scaling factor applied to the element sized based separation
distance used when performing the direct or bitmap intersection. The final intersection of faces is only
applied to those faces that are closer to each other than a specified distance. This distance is calculated
as the sum of the average depth of the elements on side 1 and side 2 of the interface. This factor is
applied as a scaling on the default distance. It might be necessary to adjust this factor if the normal
element depth on the two interfaces sides varies a lot, or side 1 and 2 of the interface are separated
by thin regions (for example, thin fin type geometries).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
211
212
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 21: Output Control
The Output Control panel is used to manage the way files are written by the solver. If a transient simulation is running, you can control which variables will be written to transient results files, and how
frequently files will be created. Results can be written at particular stages of the solution by writing
backup files after a specified number of iterations. These backup files can be loaded into CFD-Post so
that the development of the results can be examined before the solution is fully converged. Monitor
data can also be written to track the solution progress. Particle tracking data can be written for post
processing in CFD-Post. Surface data can be exported.
This chapter describes:
21.1. User Interface
21.2. Working with Output Control
21.1. User Interface
The Output Control dialog box is accessible by clicking Output Control
, by selecting Insert >
Solver > Output Control, or by editing the Output Control object listed in the tree view under
Simulation > Solver. You can also edit the CCL directly to change the object definition; for details,
see Using the Command Editor (p. 335).
The topics in this section include:
•
Results Tab (p. 213)
•
Backup Tab (p. 214)
•
Transient Results Tab (p. 215)
•
Transient Statistics Tab (p. 217)
•
Monitor Tab (p. 219)
•
Particles Tab (p. 224)
•
Export Results Tab (p. 228)
•
Common Settings (p. 230)
21.1.1. Results Tab
The Results tab for the Output Control object contains settings that control the content of the
results file that is written at the end of a solver run. In the case of a transient run, the results file contains
information from the last timestep.
21.1.1.1. Option
See Option (p. 230).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
213
Chapter 21: Output Control
21.1.1.2. File Compression
See File Compression (p. 230).
21.1.1.3. Output Variable List
See Output Variables List (p. 231).
21.1.1.4. Output Equation Residuals Check Box
See Output Equation Residuals Check Box (p. 231).
21.1.1.5. Output Boundary Flows Check Box
See Output Boundary Flows Check Box (p. 231).
21.1.1.6. Output Variable Operators Check Box
See Output Variable Operators Check Box (p. 231).
21.1.1.7. Extra Output Variables List
When the Extra Output Variables List is selected, you can specify any variable that is not included in
the results file by default. For more details, see Variables in ANSYS CFX in the CFX Reference Guide.
21.1.1.8. Output Particle Boundary Vertex Fields Check Box
See Output Particle Boundary Vertex Fields Check Box (p. 231).
21.1.2. Backup Tab
The Backup tab contains settings that specify the content of backup files, and the timesteps at which
the files are written. The purpose of the backup file is to ensure that a solver run can be restarted.
Backup files can be used to restart the simulation from the point where the error occurred, saving time
and computational resources.
21.1.2.1. List Box
This list box is used to select Backup Results objects for editing or deletion. Backup Results
objects can be created or deleted with the icons that appear beside the list box.
The union of all requested backup file content, across all Backup Results objects applicable for a
given iteration, is written as a single backup file for that iteration. If no backup file content is specified
for a given iteration in any Backup Results object, then no backup file is written for that iteration.
21.1.2.2. [Backup Results Name]
21.1.2.2.1. Option
See Option (p. 230).
214
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
21.1.2.2.2. File Compression
See File Compression (p. 230).
21.1.2.2.3. Output Variables List
See Output Variables List (p. 231).
21.1.2.2.4. Output Equation Residuals Check Box
See Output Equation Residuals Check Box (p. 231).
21.1.2.2.5. Output Boundary Flows Check Box
See Output Boundary Flows Check Box (p. 231).
21.1.2.2.6. Output Variable Operators Check Box
See Output Variable Operators Check Box (p. 231).
21.1.2.2.7. Extra Output Variables List
When the Extra Output Variables List is selected, you can specify any variable that is not included in
the results file by default. For more details, see Variables in ANSYS CFX in the CFX Reference Guide.
21.1.2.2.8. Output Particle Boundary Vertex Fields Check Box
See Output Particle Boundary Vertex Fields Check Box (p. 231).
21.1.2.2.9. Include Tracks of One-way Coupled Particles Check Box
Select or clear the check box to include or exclude tracks of one-way coupled particles to be written
to backup files. This option is available only for cases that involve one-way coupled particles. For details,
see Particle Fluid Pair Coupling Options in the CFX-Solver Modeling Guide.
21.1.2.2.10. Output Frequency: Option
See Output Frequency Options (p. 232).
21.1.3. Transient Results Tab
The Trn Results tab for the Output Control object contains settings that specify the content of
transient results files, and the timesteps at which the files are written. Each transient results file contains
results for a particular timestep. The transient results files are written in addition to the full results file
that will be written at the end of the transient simulation.
The settings on the Transient Results tab are analogous to those on the Backup tab; for details, see
Backup Tab (p. 214).
21.1.3.1. List Box
This list box is used to select Transient Results objects for editing or deletion. Transient
Results objects can be created or deleted with the icons that appear beside the list box.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
215
Chapter 21: Output Control
Only one transient results file is written at a given time regardless of how many transient results file
objects exist. Each Transient Results object will add information to the transient results file for
that timestep. Thus, the resulting transient results file is a union of the data requested by all Transient
Results objects for that timestep.
21.1.3.2. [Transient Results Name]
21.1.3.2.1. Option
See Option (p. 230).
21.1.3.2.2. File Compression
See File Compression (p. 230).
21.1.3.2.3. Output Variables List
See Output Variables List (p. 231).
21.1.3.2.4. Include Mesh
When the Selected Variables option is selected, the Include Mesh check box will be selected, in which
case the mesh data will be written to the results file. Using the Include Mesh option will allow for post
processing of the results file and will make restarting possible.
21.1.3.2.5. Output Equation Residuals Check Box
See Output Equation Residuals Check Box (p. 231).
21.1.3.2.6. Output Boundary Flows Check Box
See Output Boundary Flows Check Box (p. 231).
21.1.3.2.7. Output Variable Operators Check Box
See Output Variable Operators Check Box (p. 231).
21.1.3.2.8. Extra Output Variables List
When the Extra Output Variables List is selected, you can specify any variable that is not included in
the results file by default. For more details, see Variables in ANSYS CFX in the CFX Reference Guide.
21.1.3.2.9. Output Particle Boundary Vertex Fields Check Box
See Output Particle Boundary Vertex Fields Check Box (p. 231).
21.1.3.2.10. Output Frequency
See Output Frequency Options (p. 232).
21.1.3.3. Transient Blade Row Results
Transient Blade Row Results settings are available when there is at least one disturbance defined in
the details view of the Transient Blade Row Models object.
216
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
You can control the output of variables related to the Transient Blade Row model via the following
settings:
•
Option
Choose the level of output: Essential, Selected Variables, or None.
•
File Compression
Choose the level of file compression as a trade-off between file size and speed.
•
Output Variables List
This setting is required for the Selected Variables option.
You can multi-select variables from a list (using the Ctrl key) to have them added to the output.
•
Extra Output Variables List
This setting is available for the Essential option.
You can multi-select variables from a list (using the Ctrl key) to have them added to the output.
Data compression is based on a Fourier series. The Data Compression settings control the number of
Fourier coefficients to store in the output and the portion of the simulation over which these coefficients
are accumulated.
You can specify the number of Fourier coefficients to be stored in the output.
The Start Accumulating setting controls when the Fourier Coefficients should start being accumulated.
The available options are:
•
Last Period
The solver accumulates Fourier Coefficients during the last period of the run.
Note
Once you have specified the output for transient blade row results, there is no need to create
intermediate transient results files.
For instructions on setting up and using Transient Blade Row models, see Transient Blade Row Modeling
in the CFX-Solver Modeling Guide.
21.1.4. Transient Statistics Tab
The Trn Stats tab for the Output Control object contains settings that specify the transient statistics
data to be included in the results files; for details, see Working with Transient Statistics (p. 233).
21.1.4.1. List Box
This list box is used to select Transient Statistics objects for editing or deletion. Transient
Statistics objects can be created or deleted with the icons that appear beside the list box.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
217
Chapter 21: Output Control
21.1.4.2. [Transient Statistics Name]
21.1.4.2.1. Option
The following statistics are evaluated at each node over the history of the simulation:
•
Arithmetic Average
•
Minimum
•
Maximum
•
Standard Deviation
•
Root Mean Square
•
Full
21.1.4.2.2. Output Variables List
See Output Variables List (p. 231).
If a selected output variable is a vector or a tensor, the selected operation Option is applied to each
component of the variable separately. The result for each component is included in the results file. For
example, if Velocity is selected as a variable, using the Maximum option, the results file will include
the maximum value of each of the three velocity components. Note that the maximum value of each
of the components will likely have occurred at different times during the simulation. Also note that the
magnitude of the resulting velocity components will not be the same as the maximum of the velocity
magnitude (the latter can be determined by using the Maximum option for an additional variable
defined to be the velocity magnitude).
21.1.4.2.3. Start Iteration List Check Box
This check box determines whether or not a Start Iteration List is used. If this check box is cleared,
statistics will start (or continue, for restart runs) accumulation during the first timestep of the current
run.
21.1.4.2.3.1. Start Iteration List Check Box: Start Iteration List
Enter a comma-separated list of iteration numbers corresponding to the variables selected in the Output
Variables List. If the start iteration list contains fewer entries than the Output Variables List, then the
final start iteration in the list is applied for all remaining output variables.
The start iteration for a given transient statistic specifies the timestep index at which statistic accumulation begins. Prior to that timestep, statistics are initialized, as outlined in Working with Transient Statistics (p. 233).
Note
In the case of restarted transient runs, iteration numbers are interpreted as the total accumulated timestep index rather than the index for the current run.
21.1.4.2.4. Stop Iteration List Check Box
This check box determines whether or not a Stop Iteration List is used. If this check box is cleared, the
statistics will continue accumulation until the end of the run.
218
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
21.1.4.2.4.1. Stop Iteration List Check Box: Stop Iteration List
Enter a comma-separated list of iteration numbers corresponding to the variables selected in the Output
Variables List. If the stop iteration list contains fewer entries than the Output Variables List, then the
final stop iteration in the list is applied for all remaining output variables.
The stop iteration for a given transient statistic specifies the timestep index at which statistic accumulation ceases. After that timestep, statistics are simply not modified.
Note
In the case of restarted transient runs, start and stop iterations are interpreted as the total
accumulated timestep index rather than the index for the current run.
21.1.5. Monitor Tab
The Monitor tab for the Output Control object contains settings that specify monitor output. The
following types of information can be monitored as a solution proceeds:
•
Primitive or derived solution variables
•
Fluid Properties
•
Expressions.
When monitoring expressions, the expression must evaluate to a single number; for details, see Working
with Monitors (p. 235).
21.1.5.1. Monitor Objects Check Box
This check box determines whether or not monitor data is generated as a solution proceeds. If it is selected, the following settings are available:
21.1.5.1.1. Monitor Coeff. Loop Convergence
(applies only for transient cases)
This check box determines whether or not monitor data is output within coefficient (inner) loops. Regardless of the setting, data will be output for each timestep.
21.1.5.1.2. Monitor Balances: Option
•
Full
Mass, Momentum, and other balances are written to the solver monitor file.
•
None
21.1.5.1.3. Monitor Forces: Option
•
Full
Forces and moments on wall boundaries are written to the solver monitor file.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
219
Chapter 21: Output Control
It is important to note that these forces and moments do not include reference pressure effects.
You can include reference pressure effects in the force calculation by setting the expert parameter
include pref in forces = t.
It is also important to note that for rotating domains in a transient run, forces and moments on
wall boundaries are evaluated in the reference frame fixed to the initial domain orientation. These
quantities are not influenced by any rotation that might occur during a transient run or when a
rotational offset is specified. However, results for rotating domains in a transient run may be in the
rotated position (depending on the setting of Options in CFD-Post) when they are subsequently
loaded into CFD-Post for post-processing.
•
None
21.1.5.1.4. Monitor Residuals: Option
•
Full
RMS/max residuals are written to the solver monitor file.
•
None
21.1.5.1.5. Monitor Totals: Option
•
Full
Flow and source totals (integrals over boundaries) are written to the solver monitor file.
•
None
21.1.5.1.6. Monitor Particles: Option
•
Full
If Lagrangian Particle Tracking information is included in the simulation, force, momentum, and
source data for particles are written to the solver monitor file.
•
None
21.1.5.1.7. Efficiency Output Check Box
This check box determines whether or not the device efficiency can be monitored in CFX-Solver Manager.
When selected it also activates field efficiency output to CFD-Post. If activated, the following information
must be specified:
21.1.5.1.7.1. Inflow Boundary
A single boundary condition region of type INLET.
21.1.5.1.7.2. Outflow Boundary
A single boundary condition region of type OUTLET.
21.1.5.1.7.3. Efficiency Type
Choose between Compression, Expansion, and Both Compression and Expansion.
For more information, see Activating Efficiency Output
220
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
21.1.5.1.7.4. Efficiency Calculation Method
For each of the efficiency types, two efficiency calculation options are possible: Total to Total and Total
to Static.
For more information, see Isentropic Efficiency and Total Enthalpy
21.1.5.1.8. Monitor Points And Expressions List Box
This list box is used to select monitor objects for editing or deletion. Monitor objects can be created or
deleted with the icons that appear beside the list box.
21.1.5.1.8.1. Monitor Points and Expressions: [Monitor Name]: Option
•
Cartesian Coordinates
Monitor point data includes variable values at the node closest to the specified point. A crosshair
will be displayed in the viewer to indicate the monitored node.
•
Cylindrical Coordinates
Specify the monitor point location in terms of Position Radial Comp., Position Theta Comp., and
Position Axial Comp. values.
Monitor point data includes variable values at the node closest to the specified point. A crosshair
will be displayed in the viewer to indicate the monitored node.
Note
This option disables the ability to specify the points by picking in the Viewer.
•
Expression
An expression is monitored.
21.1.5.1.8.2. Monitor Points and Expressions: [Monitor Name]: Output Variables List
(applies only when Option is set to Cartesian Coordinates)
Select the variables to monitor.
Tip
Hold the Ctrl key when clicking to select multiple variables.
21.1.5.1.8.3. Monitor Points and Expressions: [Monitor Name]: Cartesian Coordinates
(applies only when Option is set to Cartesian Coordinates)
Enter coordinates for the point location to monitor.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
221
Chapter 21: Output Control
Tip
After you click a coordinate entry area, all of the coordinate entry areas turn yellow to show
that you are in Picking mode. You can then select locations from the viewer using the mouse.
To manipulate the object in the viewer while in Picking mode, use the viewer icons (rotate,
pan, zoom) in the toolbar. You can end Picking mode by changing the keyboard focus (by
clicking in another field, for example).
21.1.5.1.8.4. Monitor Points and Expressions: [Monitor Name]: Cylindrical Coordinates
(applies only when Option is set to Cylindrical Coordinates)
Enter coordinates for the point location to monitor in terms of Position Radial Comp., Position Theta
Comp., and Position Axial Comp. values.
Note
This option disables the ability to specify the points by picking in the Viewer.
21.1.5.1.8.5. Monitor Points and Expressions: [Monitor Name]: Expression Value
(applies only when Option is set to Expression)
Enter a CEL expression that evaluates to a single number that is to be monitored.
21.1.5.1.8.6. Monitor Points and Expressions: [Monitor Name]: Coord Frame Check Box
Determines whether the coordinate frame of the monitor point is specified or left at the default of
Coord 0. For a monitor point that uses Cartesian or cylindrical coordinates, the coordinate frame is
used to interpret the specified coordinates. For a monitor point that uses an expression, the coordinate
frame affects all CEL functions that are used in the expression and that return the component of a
vector (for example, force_x()).
21.1.5.1.8.7. Monitor Points and Expressions: [Monitor Name]: Coord Frame Check Box: Coord Frame
Set the coordinate frame used for the monitor point or expression; for details, see Coordinate Frames
in the CFX-Solver Modeling Guide.
21.1.5.1.8.8. Monitor Points and Expressions: [Monitor Name]: Domain Name Check Box
Determines whether the specified Cartesian coordinates are restricted to a particular domain.
21.1.5.1.8.9. Monitor Points and Expressions: [Monitor Name]: Domain Name Check Box: Domain
Name
Set the domain name to which the specified Cartesian coordinates will be restricted.
21.1.5.1.9. Radiometer: Frame Overview
(applies only when using the Discrete Transfer or Monte Carlo thermal radiation model)
A radiometer is a user defined point in space that monitors the irradiation heat flux (not incident radiation) arriving at the required location. The user specification involves much more than just the location
222
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
of the sensor, as it also requires the viewing direction, its temperature and some numerical controls for
each particular sensor.
By default, radiometers are ideal and the efficiency factor is 1.
A cyan arrow with a cross-hair is used to denote the location of each sensor in the viewer.
21.1.5.1.10. Radiometer: List Box
This list box is used to select Radiometer objects for editing or deletion. Radiometer objects can
be created or deleted with the icons that appear beside the list box.
21.1.5.1.10.1. Radiometer: [Radiometer Name]: Option
•
Cartesian Coordinates
21.1.5.1.10.2. Radiometer: [Radiometer Name]: Cartesian Coordinates
Enter Cartesian coordinates that describe the location of the radiometer. These coordinates are interpreted
in the coordinate frame associated with the radiometer. For details, see Coordinate Frames (p. 255) and
also Coordinate Frames in the CFX-Solver Modeling Guide.
21.1.5.1.10.3. Radiometer: [Radiometer Name]: Temperature
Enter the temperature of the radiometer.
21.1.5.1.10.4. Radiometer: [Radiometer Name]: Quadrature Points
Enter the number of rays used for ray tracing from the radiometer.
21.1.5.1.10.5. Radiometer: [Radiometer Name]: Coord Frame Check Box
This check box determines whether the coordinate frame used to interpret the location and direction
specifications of the radiometer will be specified or left at the default of Coord 0.
21.1.5.1.10.6. Radiometer: [Radiometer Name]: Coord Frame Check Box: Coord Frame
Select a coordinate frame to interpret location and direction specifications of the radiometer. For details,
see Coordinate Frames (p. 255) and also Coordinate Frames in the CFX-Solver Modeling Guide.
21.1.5.1.10.7. Radiometer: [Radiometer Name]: Diagnostic Output Level Check Box
This check box determines whether the diagnostic output level will be specified or left at the default
of 0.
21.1.5.1.10.8. Radiometer: [Radiometer Name]: Diagnostic Output Level Check Box: Diagnostic
Output Level
Enter a number greater than zero. The CFX-Solver will write the ray traces to a series of polylines in a
.csv file that can be visualized in CFD-Post. This can be used to determine if the number of quadrature
points is optimal.
21.1.5.1.10.9. Radiometer: [Radiometer Name]: Direction: Option
•
Cartesian Components
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
223
Chapter 21: Output Control
21.1.5.1.10.10. Radiometer: [Radiometer Name]: Direction: X Component,Y Component, Z Component
(applies only when Monitor Objects check box: Radiometer: [Radiometer Name]: Direction: Option
is set to Cartesian Components)
Enter a numerical quantity or CEL expression for each Cartesian component of a direction vector that
represents the orientation of the radiometer.
21.1.6. Particles Tab
The Particles tab for the Output Control object contains settings that specify whether the particle
data is recorded, and details of how the data is collected and recorded.
This tab is available only when the morphology option is set to Particle Transport Fluid or
Particle Transport Solid in CFX-Pre; for details, see Basic Settings Tab (p. 107).
The particle data is initially written to particle track files, which contain a specified level of detail about
particles involved in your simulation. The files are written to the directory with the same name as your
current run. An option on the Particles tab controls whether or not the track files are retained after
their data is copied into the final results file (and any backup results files).
21.1.6.1. Particle Track File Check Box
This check box determines whether or not to customize the type and amount of particle track data recorded in the results file.
21.1.6.1.1. Option
•
All Track Positions (default)
Point data is collected for all track positions, as determined by the Track Positions setting.
•
Specified Position Interval
Point data is collected for a subset of all track positions. The entire set of track positions is determined by the Track Positions setting. The subset is controlled by the Interval setting. For example,
if Track Position Interval is left at its default value of 1, then the result is the same as setting Option
to All Track Positions. Setting Interval to 2 will cause point data to be collected for every second
track position; setting Interval to 3 will cause point data to be collected for every third track position,
and so on.
•
Specified Distance Spacing
Point data is collected for evenly-spaced points along each track. The spacing is controlled by this
parameter, and represents a physical distance.
•
Specified Time Spacing
Point data is collected for points along each track with the points spaced by time according to this
parameter. The physical distance between data collection points is therefore a function of the
particle velocity along each track.
•
None
This option can be used to avoid writing any track information. This might be useful if you are not
interested in particle tracks or want to avoid the additional disk space required to store the tracks.
224
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
If this option is set, no tracks will be available in CFD-Post. In contrast to the track file information,
sources are required for a clean re-start of a particle case and must be written to the results file.
Note
For a transient run, final particle positions are always added to the track information, and
therefore can be seen at the end of a run.
21.1.6.1.2. Track Positions Check Box
(applies only when Particle Track File Check Box: Option is set to All Track Positions or
Specified Position Interval)
This check box determines whether the Track Positions setting will be specified, or left at the default
value: Element Faces.
21.1.6.1.3. Track Positions Check Box: Track Positions
•
Control Volume Faces
Points are written each time a sub-control volume boundary is crossed. This produces the more
precise and larger track files than the other option.
•
Element Faces
Points are written to the track file each time a particle crosses the boundary of an element.
21.1.6.1.4. Interval
(applies only when Particle Track File Check Box: Option is set to Specified Position Interval)
Enter an integer that specifies the spacing (in terms of points) between points along the tracks.
21.1.6.1.5. Track Distance Spacing
(applies only when Particle Track File Check Box: Option is set to Specified Distance Spacing)
Enter a numerical quantity that specifies the physical distance interval between successive points on
the track. Data will be collected only for those points.
21.1.6.1.6. Track Time Spacing
(applies only when Particle Track File Check Box: Option is set to Specified Time Spacing)
Enter a numerical quantity that specifies the physical time interval between successive points on the
track. Data will be collected only for those points.
21.1.6.1.7. Track Printing Interval Check Box
This check box determines whether the Track Printing Interval setting will be specified, or left at the
default value: 1.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
225
Chapter 21: Output Control
21.1.6.1.8. Track Printing Interval Check Box: Interval
Output data is collected for every nth particle track, where n is the specified number.
21.1.6.1.9. Keep Track File Check Box
Determines whether or not the track files are kept. When the track files are kept, they can be found
below the working directory in a directory that has the same name as the run. For example, for the first
solution of dryer.def, the track files are kept in a directory called dryer_001.
The data will be copied into the results file regardless of whether or not the track files are kept. CFDPost can extract the track file data from the results file for post processing.
21.1.6.1.10. Track File Format Check Box
Determines whether the track file format will be specified, or left at the solver default value: Unformatted.
The track file will remain in the working directory after finishing a run only if you select the Keep Track
File option to force the solver to not delete it.
21.1.6.1.11. Track File Format Check Box: Track File Format
•
Formatted
Formatted track files are in human-readable ASCII format but take up much more disk space than
unformatted track files.
The general structure of formatted ASCII track files will print the Number of Particle Positions in a
Block at the top of the file preceding repetitions of the following:
Particle Track Number
X Position
Y Position
Z Position
Traveling Time
Traveling Distance
Particle Diameter
Particle Number Rate
Particle Mass Fraction Component 1
Particle Mass Fraction Component 2
....
Particle Mass Fraction Component n
Particle U Velocity
Particle V Velocity
Particle W Velocity
Particle Temperature
Particle Mass
Note
Particle Mass Fraction Component 1- n only appear for multi-component particle materials and Particle Temperature only appears when heat transfer is activated.
•
Unformatted
Unformatted track files are written in a non-readable, binary, format.
226
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
21.1.6.2. Transient Particle Diagnostics
This section is available for transient simulations using particle tracking and enables you to output
various particle data; for details, see Transient Particle Diagnostics in the CFX-Solver Modeling Guide.
21.1.6.3. Transient Particle Diagnostics: List Box
Shows the current Transient Particle Diagnostics outputs. You can click
output file or click
to create a new diagnostics
to delete an existing one.
21.1.6.4. Transient Particle Diagnostics: [Transient Particle Diagnostics Name]
21.1.6.4.1. Option
•
Particle Penetration
•
Total Particle Mass
•
User Defined - This option can be used to specify a user-defined Diagnostic Routine to evaluate the
diagnostics information based on particle variables specified in Particle Variables List. Optionally, you
can also select the Monitored Values List check box and specify a comma-separated list of names for
monitored values. For details, see User Diagnostics Routine in the CFX-Solver Modeling Guide.
21.1.6.4.2. Particles List
Select particles to be used for output from the drop-down list, or click
List dialog box.
and select from the Particles
21.1.6.4.3. Spray Mass Frac.
The fraction of the total spray mass contained within an imaginary cone, the half-angle of which is the
spray angle. The cone tip is at the point of injection and the cone axis is parallel to the direction of injection.
21.1.6.4.4. Penetration Origin and Direction: Option
•
Specified Origin and Direction
21.1.6.4.5. Penetration Origin and Direction: Injection Center
Enter the Cartesian coordinates of the center of injection.
21.1.6.4.6. Penetration Origin and Direction: Injection Direction
21.1.6.4.6.1. Option
•
Cartesian Components
Specify the Cartesian components (Direction X Comp., Direction Y Comp., and Direction Z Comp.)
of the injection direction.
21.1.6.4.7. Axial Penetration: Option
•
Axial Penetration
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
227
Chapter 21: Output Control
See Spray Penetration in the CFX-Solver Modeling Guide in Transient Particle Diagnostics in the CFXSolver Modeling Guide for details.
•
None
21.1.6.4.8. Radial Penetration: Option
•
Radial Penetration
See Spray Penetration in the CFX-Solver Modeling Guide in Transient Particle Diagnostics in the CFXSolver Modeling Guide for details.
•
None
21.1.6.4.9. Normal Penetration: Option
•
Normal Penetration
See Spray Penetration in the CFX-Solver Modeling Guide in Transient Particle Diagnostics in the CFXSolver Modeling Guide for details.
•
None
21.1.6.4.10. Spray Angle: Option
•
Spray Angle
See Spray Penetration in the CFX-Solver Modeling Guide in Transient Particle Diagnostics in the CFXSolver Modeling Guide for details.
•
None
21.1.6.4.10.1. Spray Angle: Spray Radius at Penetration Origin Check Box
Enable to specify a spray radius for the penetration origin.
21.1.6.4.10.2. Spray Angle: Spray Radius at Penetration Origin Check Box: Spray Radius
Enter a penetration origin spray radius.
21.1.7. Export Results Tab
The Export Results tab for the Output Control object is used to specify export files; for details, see
Working with Export Results (p. 237).
Note
The flow solver Export Results supports "Stationary" wall boundary conditions only when
mesh motion is activated.
21.1.7.1. List Box
This list box is used to select Export Results objects for editing or deletion. Export Results
objects can be created or deleted with the icons that appear beside the list box.
228
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
21.1.7.2. [Export Name]: Export Format
The Export Format check box determines whether the export format will be specified, or left at its
default of CGNS. Currently, the only option is CGNS.
21.1.7.2.1. Filename Prefix Check Box
This check box determines whether or not a user-specified prefix is used in the filenames of exported
files. By default, CFX-Solver will use the object name as the filename prefix. For details, see File Naming
Conventions (p. 237).
21.1.7.2.2. Filename Prefix Check Box: Filename Prefix
Specify a prefix to use in the filenames of exported files.
21.1.7.3. [Export Name]: Export Frequency
21.1.7.3.1. Option
•
Time List
See Time List (p. 232).
•
Time Interval
See Time Interval (p. 232).
•
Iteration List
See Iteration List (p. 232).
•
Iteration Interval
See Iteration Interval (p. 232).
•
Every Iteration
21.1.7.4. [Export Name]: Export Surface
21.1.7.4.1. List Box
This list box is used to select Export Surface objects for editing or deletion. Export Surface
objects can be created or deleted with the icons that appear beside the list box. Solution fields are required either on individual 2D boundary regions or on composite boundary regions.
21.1.7.4.2. [Export Surface Name]: Option
•
Selected Variables
•
Acoustic Dipole/Acoustic Rotating Dipole
21.1.7.4.3. [Export Surface Name]: Output Boundary List
See Output Boundary List and Output Region Naming (p. 237).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
229
Chapter 21: Output Control
21.1.7.4.4. [Export Surface Name]: Output Variables List
(applies only when Option is set to Selected Variables). For details, see Output Variables List (p. 231).
21.1.7.4.5. [Export Surface Name]: Output Nodal Area Vectors Check Box
(applies only when Option is set to Selected Variables)
Select this check box, and the Value check box contained within Output Nodal Area Vectors, when
exporting acoustic data for LMS noise analysis.
21.1.8. Common Settings
21.1.8.1. Option
•
Selected Variables
Selected vertex fields are written to the results file. The fields are chosen from the Output Variables
List. No restart is possible from these files.
•
Smallest (not available on the Results tab)
Mesh data and all solution vertex fields are written. A restart is possible from these files, but the
restart will not be “clean” (you can expect a temporary increase in residual values).
•
Essential
The smallest file that preserves a clean restart is written. This includes data written in the Smallest
category and the following:
•
–
GGI control surface fields
–
Boundary face solution arrays
–
Mass flow data fields
Standard
This contains data written in the Essential category and the following:
•
–
Hybrid fields
–
Post processing fields
None
Used when no output of results is required (for example, during solver performance benchmarking).
21.1.8.2. File Compression
•
None
This offers no compression.
•
Default
This is a compromise between disk space and processing load.
•
Best Speed Least Compression
•
Low Speed Most Compression
230
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
You may want to increase the compression level for large backup files, or if you do not have much disk
space.
21.1.8.3. Output Variables List
Allows you to select the output variables to write to the results file. Select the desired variables from
the list or click the
icon to select from a list of all variables. Output Variable List is only available
when Selected Variables is the option selected.
21.1.8.4. Output Equation Residuals Check Box
When Output Equation Residuals is set to All, the equation residuals for all equations are written to
the results file for steady state solutions. The residuals can then be viewed in CFD-Post. They appear as
ordinary variables available from the full list of variables. This parameter replaces the expert parameter
output eq residuals.
21.1.8.5. Output Boundary Flows Check Box
When Output Boundary Flows is set to All, equation flows, including mass flows, are written to the
file you have set up. These flows enable accurate evaluations of forces, heat flows, and mass flow related
calculations in CFD-Post. These flows are always written for Standard backup/results and transient
files. They are not written for Selected Variables and Smallest transient files, unless the Output
Boundary Flows parameter is set to All.
21.1.8.6. Output Variable Operators Check Box
When Output Variable Operators is set to All, you get all available operators that the solver has
calculated (for example, gradients, High Resolution betas) for the variables in the Output Variables
List. This option only applies to minimal transient results files, selected variables, backup results and
results files. These operators are always written for Standard files, but may also be written for Selected Variables and Smallest files by setting this parameter to All.
21.1.8.7. Output Particle Boundary Vertex Fields Check Box
For cases with particles, when Output Particle Boundary Vertex Fields is selected, the following
boundary vertex fields are written:
•
•
Inlets, outlets, openings and interfaces:
–
Mass flow density
–
Momentum flow density
–
Energy flow density
Walls:
–
Mass flow density
–
Stress
–
Erosion rate density.
For transient cases, the following additional boundary vertex fields are written:
•
Inlets, outlets, openings and interfaces:
–
Time integrated mass flow density
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
231
Chapter 21: Output Control
•
–
Time integrated momentum flow density
–
Time integrated energy flow density
Walls:
–
Time integrated mass flow density
–
Time integrated erosion rate density.
For additional details, see Particle Boundary Vertex Variables in the CFX Reference Guide
21.1.8.8. Output Frequency Options
This determines how often backup and transient results files are written during a run.
21.1.8.8.1. Timestep Interval
Enter a number that specifies the number of timesteps between the writing of each results file.
21.1.8.8.2. Timestep List
Enter a comma-separated list of timestep numbers that specifies the timesteps at which files are written.
21.1.8.8.3. Time Interval
Enter a number that specifies the simulation time interval between the writing of each file. The simulation
time interval is added to a running total that starts at the simulation start time. An iteration within half
a timestep of the current total has a file written.
21.1.8.8.4. Time List
Enter a comma-separated list of simulation times that specifies the iterations at which files are written.
21.1.8.8.5. Every Timestep
No further input is needed. A backup or transient results file is written for every timestep in a transient
simulation.
21.1.8.8.6. Every Iteration
No further input is needed. A backup or transient results file is written for every iteration.
21.1.8.8.7. Iteration Interval
Enter a number that specifies the number of iterations between the writing of each file.
21.1.8.8.8. Iteration List
Enter a comma-separated list of iteration numbers that specifies the iterations at which files are written.
21.1.8.8.9. Wall Clock Time Interval
(Only available for backup files)
Enter a number that specifies the wall clock time interval between the writing of each backup file.
232
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with Output Control
This is used to create backup files every so often in real time. For example, on an overnight simulation
you might choose to have a backup file created every two hours, regardless of how many iterations or
timesteps had been performed.
21.1.8.8.10. Coupling Step Interval
(Only available for ANSYS Multi-field runs). Enter a number that specifies the number of coupling steps
(multi-field timesteps) between the writing of each file. Note that if you are using CFX-Pre in ANSYS
MultiField mode to set up the multi-field part of an ANSYS Multi-field run, then selecting this option
has implications for how often the ANSYS Solver writes its results, in addition to specifying how often
CFX should write results. For details, see The Processing Step in the CFX-Solver Manager User's Guide.
21.1.8.8.11. Every Coupling Step
(Only available for ANSYS Multi-field runs). This is used to create a results file every coupling step (multifield timestep). Note that if you are using CFX-Pre in ANSYS MultiField mode to set up the multifield part of an ANSYS Multi-field run, then selecting this option has implications for how often the
ANSYS Solver writes its results, in addition to specifying how often CFX should write results. For details,
see The Processing Step in the CFX-Solver Manager User's Guide.
21.1.8.8.12. None
No results files will be written. You might choose this option to temporarily turn off writing backup or
transient files but keeping the definition of what to include in the files so that you can easily re-enable
them.
21.2. Working with Output Control
The following topics will be discussed:
•
Working with Transient Statistics (p. 233)
•
Working with Monitors (p. 235)
•
Working with Export Results (p. 237)
21.2.1. Working with Transient Statistics
This section describes the generation and output of running statistics for solution variables. The available
statistics are arithmetic average, minimum, maximum, root-mean-square (RMS) and standard deviation.
This follows from the same statistical theory that is used to determine statistical Reynolds Stresses, for
example,
′ ′ in turbulence modeling.
21.2.1.1. Statistic Initialization and Accumulation
Arithmetic averages are initialized using the solution values. RMS values are initialized using the absolute
value of the solution values. Each of these statistics is calculated recursively by adding timestep-weighted
solution values from the latest timestep to the accumulating statistic.
Minimum and maximum statistics are initialized using the solution values, and are updated as new extremes are found.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
233
Chapter 21: Output Control
Standard deviations are initialized with a value of zero. The standard deviation is essentially an RMS of
the difference between the latest solution value and the running arithmetic average. If this difference
is written as ′, then the mean of the squared difference follows from the same statistical theory that
is used to determine statistical Reynolds Stresses, for example, ′ ′ in turbulence modeling, and can
be calculated as:
′ ′ = − =
− The required RMS and arithmetic average statistics are automatically activated when the standard deviation is requested. It is also important to note that an error may be introduced in evaluating the
standard deviation if it is calculated before either of the mean or RMS statistics. This error varies approximately with the inverse of the number of data (that is, the number of timesteps) used to calculate the
statistics. For instance, this error should be less than approximately 1% once the statistics contain more
than 100 pieces of data.
21.2.1.2. Statistics as Variable Operators
Transient statistics are operators that act on variables (both conservative and hybrid values) identified
in the Output Variables List. Like other variable operators, the data written to results files have names
like <variable>.<statistic> where <variable> is the name of the specified variable and <statistic>
is one of the following:
•
Trnmin (Minimum)
•
Trnmax (Maximum)
•
Trnavg (Arithmetic average)
•
Trnrms (Root mean square)
•
Trnsdv (Standard deviation)
Tip
To output transient statistics for intermediate results, be sure to select the Output Variable
Operators check box on the Transient Results tab.
Choose the Full option if all variable operators are desired.
A significant consequence of treating transient statistics as operators is that only one instance of a
<variable>.<statistic> exists during the entire simulation. For example, even if multiple transient
statistics objects containing the arithmetic average of velocity are requested, only one statistic will ever
exist. The potential for specifying different start (stop) iterations for these transient statistics objects is
addressed by using the earliest (latest) value specified; that is, statistics are accumulated over the largest
range of timesteps possible as defined by the start and stop iterations for all transient statistics objects.
Note
If you want to re-initialize a given statistic (that is, remove the history from the statistic), you
must shut down and restart the simulation with a new start (stop) iteration. This step is required to ensure that the new statistic accumulation interval is not included when searching
for the earliest and latest start and stop iteration values, respectively.
234
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with Output Control
21.2.1.3. Using Statistics with Transient Rotor-Stator Cases
You can use transient statistics to examine the convergence of a transient/rotor stator case. This is done
by obtaining averaged variable data over the time taken for a blade to move through one pitch. By
comparing consecutive data sets, you can examine if a pseudo steady-state situation has been reached.
Variable data averaged from integer pitch changes should be the same if convergence has been achieved.
Each of the variables that are created by the CFX-Solver can be used in CFD-Post to create plots or
perform quantitative calculations.
21.2.2. Working with Monitors
21.2.2.1. Setting up Monitors
1.
Click Output Control
or select Insert > Solver > Output Control from the main menu.
The Output Control dialog box will appear.
2.
Click the Monitor tab.
3.
Select Monitor Objects.
4.
Select which variables to monitor (Balances, Forces, Residuals, Totals, Particles).
By default, all of the listed quantities are monitored.
5.
Click Add new item
.
The Monitor Points and Expressions dialog box pops up to ask for the name of a new monitor
point object.
6.
Enter a name, or accept the default name, and then click OK.
The [Monitor Name] frame expands to show a set of input fields.
7.
Specify the settings for the monitor object.
8.
Add more monitor objects as desired.
9.
Click OK or Apply to set the definitions of all of the monitor objects. All monitor points will be displayed
in the viewer.
21.2.2.2. Transient/ Mesh Deformation Runs
The closest node for Cartesian coordinate is chosen for output. For a transient run or run with a moving
mesh, the closest node is identified once at the start and used for the remainder of the run. For details,
see Mesh Deformation (p. 113).
21.2.2.3. Output Information
Information on the variables to be monitored is given near the start of the .out file. In the following
example the variables Velocity and Pressure were requested for the Output Variables List in the .ccl
file.
+-----------------------------------------------------------------------+
|
User Defined Monitor Points
|
+-----------------------------------------------------------------------+
Monitor Point: my monitor point
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
235
Chapter 21: Output Control
Domain: rotor
Monitor vertex location (x,y,z):
4.101E-01, 5.703E-02, 5.263E-02
User specified location (x,y,z):
4.100E-01, 5.618E-02, 4.951E-02
Distance to user specified location:
3.231E-03
Valid variables from output variable list:
Air Ideal Gas.Velocity u
Air Ideal Gas.Velocity v
Air Ideal Gas.Velocity w
Pressure
+-----------------------------------------------------------------------+
The “Monitor vertex location” shows the actual location that is being monitored (the closest vertex to
the “User specified location”). The “Distance to user specified location” shows the difference between
the specified and actual monitoring location.
The “Output variable list” shows the full name of all variables that will be monitored.
21.2.2.4. Expression
When using the Expression option, the results of the evaluated expression are output at each iteration.
Enter an expression that evaluates to a single value at each timestep. The following are examples of
expressions that could be monitored:
•
force()@MainWall / (0.5*areaAve(density)@Inlet * areaAve(vel)@Inlet *
area()@MainWall)
•
volumeAve(CO2.mf)@Domain 1
The variable names should be preceded with the fluid name when applicable. You can view a list of
variable names in the Expression details view by right-clicking in the Definition window when editing
an expression.
21.2.2.5. Viewing Monitor Values during a Run
You can view a plot of monitor point values during a solver run. For details, see Monitors Tab in the
CFX-Solver Manager User's Guide.
21.2.2.6. Viewing Monitor Point Values after a Run
After the CFX-Solver has finished, the monitor point data (if the monitor point information is required)
is extracted from a .res file using the cfx5dfile command. The following syntax is used:
cfx5dfile <file> -read-monitor
where <file> is a CFX-Solver input or results file containing monitor point information. The output
is sent to standard output (you may want to add a redirect to write the output to a text file, for example:
cfx5dfile <file> -read-monitor > out.txt
The output is produced as a list of variable names, followed by a comma-delimited list of values that
correspond to the order of variable names. One line of these values is produced for every iteration that
has been carried out.
You can enter:
cfx5dfile -help
to obtain more information.
236
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Working with Output Control
21.2.3. Working with Export Results
The topics in this section include:
•
File Naming Conventions (p. 237)
•
Propagating Older Time Step Values (p. 237)
•
Output Boundary List and Output Region Naming (p. 237)
•
Output Variables List (p. 238)
21.2.3.1. File Naming Conventions
Each instance of an Export Results object will correspond to a particular group of files in a transient
run.
Transient data is written into a series of files, named using the form:
<prefix>_<timestep>.<extension>
•
<prefix> defaults to the Export Results object name unless you override this with the parameter
“Filename Prefix”
•
<timestep> is a string containing the timestep number
•
cgns is the only available <extension>
The mesh information (mesh coordinates and nodal area vectors, if applicable) is written into a separate
file to save disk space, because the mesh information does not change with time. The mesh file name
is of the form:
<prefix>_mesh.cgns
A link is created for each solution file (<prefix>_<timestep>.cgns) to map the mesh coordinates
to the mesh file (<prefix>_mesh.cgns). If you write your own reader, you need not open the mesh
file separately to read in the mesh coordinates for each solution file.
21.2.3.2. Propagating Older Time Step Values
When exporting results to 3rd party applications, it is possible that values from an earlier time step are
written at time steps where true data does not exist - for example at time steps where minimal results
files were requested in the solver control setup. This is done because some 3rd party software can only
successfully read exported files when a consistent number of variables exists in each file. It is up to you
to recognize that these “dummy variables” are not accurate at the particular time step.
21.2.3.3. Output Boundary List and Output Region Naming
The default behavior of this parameter is to attempt to create one composite boundary region per domain. The boundary condition patches do not have to be in the same domain so that rotating dipole
sources and regular dipole sources will be contained in the same export file if this is desired.
Each export surface object name is unique. If the export surface lies within one domain, the name of
each exported surface will simply be the Export Surface object name. If the export surface lies
across multiple domains, a region will be exported for each domain spanned by the export surface.
Such regions are named using the form "<domain name>.<export surface name>".
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
237
Chapter 21: Output Control
21.2.3.4. Output Variables List
When either of the acoustic options are selected, the output variables list is implied. For both acoustic
options, there is output for pressure on vertices and the surface mesh (x, y, z and topology). For the
rotating dipole option there is also output for nodal area vectors.
238
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 22: Transient Blade Row Models
This chapter describes the Transient Blade Row Models object that can appear in the Outline
tree.
For instructions on setting up and using Transient Blade Row models, see Transient Blade Row Modeling
in the CFX-Solver Modeling Guide.
This chapter describes:
22.1. Inserting a New Transient Blade Row Models Object
22.2.Transient Blade Row Models Tab
22.1. Inserting a New Transient Blade Row Models Object
Setting up a Transient Blade Row Model in the CFX-Solver Modeling Guide describes a procedure for inserting a Transient Blade Row Model object.
To insert a Transient Blade Row Models object:
1.
2.
Do one of the following:
•
Right-click Flow Analysis 1 (or whichever analysis is applicable) in the Outline tree, then select
Insert > Transient Blade Models from the shortcut menu.
•
Select Flow Analysis 1 (or whichever analysis is applicable) in the Outline tree, then select
Insert > Transient Blade Row Models from the main menu.
Click OK.
22.2. Transient Blade Row Models Tab
The Transient Blade Row Models tab is available after you insert the object of the same name. For
details, see Inserting a New Transient Blade Row Models Object (p. 239).
The following sections describe the settings on the Transient Blade Row Models tab
22.2.1.Transient Blade Row Model Settings
22.2.2.Transient Details
22.2.1. Transient Blade Row Model Settings
The Transient Blade Row Model > Option setting can have one of the following values:
•
None
This option disables Transient Blade Row modeling. It is useful when running transient simulations
without any transformations.
•
Profile Transformation
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
239
Chapter 22: Transient Blade Row Models
The Transient Details settings (Time Period, Time Steps, and Time Duration) must be configured.
These settings are described in Transient Details (p. 242).
•
Time Transformation
To help the solver apply the Time Transformation method to the applicable domains, you must
accurately characterize a disturbance. For details, see Time Transformation Disturbance Settings (p. 240).
The Transient Details settings (Time Period, Time Steps, and Time Duration) must be configured.
These settings are described in Transient Details (p. 242).
•
Fourier Transformation
To help the solver apply the Fourier Transformation method to the applicable domains, you must
accurately characterize a disturbance. For details, see Fourier Transformation Disturbance Settings (p. 241).
The Transient Details settings (Time Period, Time Steps, and Time Duration) must be configured.
These settings are described in Transient Details (p. 242).
22.2.1.1. Time Transformation Disturbance Settings
A given domain can receive a disturbance from:
•
An upstream or downstream domain interface that uses the Transient Rotor Stator frame
change/mixing model. For example, the wake from a blade can pass through a domain interface
and disturb the downstream domain(s).
The Time Transformation method improves solution accuracy over that of the Profile
Transformation method when there is unequal pitch between the blade row subsets on each
side of a domain interface that uses the Transient Rotor Stator frame change/mixing model.
•
Inlet or outlet (or opening) boundaries. For example, a boundary condition could use a CEL function
that depends on space and time in order to mimic the wake of an upstream blade.
The Time Transformation method can be applied to a domain that has an inlet or outlet
disturbance.
To characterize a disturbance, create a new item by clicking Add new item
, enter a unique name
for the disturbance, then specify information about the disturbance in one of the following ways:
•
Rotor Stator option
This option can be applied only when the disturbance originates from a domain interface that uses
the Transient Rotor Stator frame change/mixing model.
After selecting this option:
1.
Select a Domain Interface from the existing domain interfaces that use the Transient Rotor Stator
frame change/mixing model.
2.
For each side of the interface (Side 1 and Side 2, which correspond to the first and second sides
of the selected domain interface, respectively) specify the Option setting.
The Option setting for each side is used to determine the domain(s) to which the Time Transformation method is applied. The options for each side are:
240
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transient Blade Row Models Tab
–
Automatic
This option causes the solver to identify the domain(s) directly touching the applicable side of
the interface. This option is suitable when all the domains that are affected by the disturbance
are in contact with the applicable side of the interface.
–
Domain List
This option enables you to manually select the domain(s) that are on the applicable side of the
interface and that are affected by the disturbance. You might need to use this option if, for
example, a blade row is modeled with two domains with one being downstream of the other,
in which case you would select both domains as being on one side of the interface, even though
one of those domains does not touch the interface.
–
None
This option prevents the present disturbance (but not any other disturbances) from applying
the Time Transformation method to any domain that is on the applicable side of the interface.
For details, see Case 1: Transient Rotor Stator Single Stage in the CFX-Solver Modeling Guide.
•
Rotational Flow Boundary Disturbance option
Use this option to characterize a disturbance that originates from a boundary condition (for example,
an inlet or outlet boundary condition that is specified using one or more CEL expressions that depend on space and time).
After selecting this option:
1.
Set Domain Name to the name of the domain(s) that are affected by the disturbance.
2.
Set the Signal Motion settings:
3.
–
Setting Option to Stationary causes the signal to be stationary in the absolute (stationary)
frame of reference.
–
Setting Option to Rotating enables you to select a coordinate frame as a way of specifying
the signal motion. Any boundary using this coordinate frame will be made transient periodic
with the period calculated from the pitch and rotating speed of the signal. For details on
moving coordinate frames, see Frame Motion Settings.
Specify information about the external blade row that creates the disturbance in the External
Passage Definition settings:
–
4.
For a case with rotational periodicity, specify Passages in 360: the number of passages in 360°
of the external blade row that creates the disturbance. Also specify Passages / Component:
the number of passages in the external blade row that creates the disturbance.
For a case with rotational periodicity, the Passages in 360 and Passages / Component settings
on the domain Basic Settings tab apply.
For details, see Case 2: Flow Boundary Disturbance in the CFX-Solver Modeling Guide.
22.2.1.2. Fourier Transformation Disturbance Settings
A given domain can receive a disturbance from:
•
Inlet or outlet (or opening) boundaries. For example, a boundary condition could use a CEL function
that depends on space and time in order to mimic the wake of an upstream blade.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
241
Chapter 22: Transient Blade Row Models
The Fourier Transformation method can be applied to a domain that has an inlet or
outlet disturbance.
To characterize a disturbance, create a new item by clicking Add new item
, enter a unique name
for the disturbance, then specify information about the disturbance:
•
Rotational Flow Boundary Disturbance option
Use this option to characterize a disturbance that originates from a boundary condition (for example,
an inlet or outlet boundary condition that is specified using one or more CEL expressions that depend on space and time).
After selecting this option:
1.
Specify the Phase Corrected Intf. and Sampling Domain Intf. settings.
The Phase Corrected Intf. setting specifies the periodic GGI-only bitmap-intersection-method
interface (having rotational periodicity) to which to apply the phase shift with respect to the
sampling domain interface signal.
The Sampling Domain Intf. setting specifies the non-periodic non-frame-change GGI-only
bitmap-intersection-method interface on which the Fourier coefficients will be accumulated.
This is the interface between a pair of adjacent blades in a given component.
2.
3.
Set the Signal Motion settings:
–
Setting Option to Stationary causes the signal to be stationary in the absolute (stationary)
frame of reference.
–
Setting Option to Rotating enables you to select a coordinate frame as a way of specifying
the signal motion. Any boundary using this coordinate frame will be made transient periodic
with the period calculated from the pitch and rotating speed of the signal. For details on
moving coordinate frames, see Frame Motion Settings.
Specify information about the external blade row that creates the disturbance in the External
Passage Definition settings:
–
4.
For a case with rotational periodicity, specify Passages in 360: the number of passages in 360°
of the external blade row that creates the disturbance. Also specify Passages / Component:
the number of passages in the external blade row that creates the disturbance.
For a case with rotational periodicity, the Passages in 360 and Passages / Component settings
on the domain Basic Settings tab apply.
For details, see Case 2: Flow Boundary Disturbance in the CFX-Solver Modeling Guide.
Note
You must ensure that the disturbance is periodic in time when using the Rotational
Flow Boundary Disturbance option.
22.2.2. Transient Details
The Time Period settings are used to establish a value for the time period in which each disturbance
of interest cycles an integer number of times. The options for obtaining this number are:
•
242
Passing Period (not available for the Fourier Transformation method)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transient Blade Row Models Tab
When this option is selected, the time period is calculated automatically as:
–
For inlet disturbance cases:
The signal pitch divided by the relative velocity between the signal and the domain.
–
For transient rotor stator cases:
The result of dividing the blade pitch by the absolute value of the angular velocity of the rotor(s),
for the specified domain.
Note that the blade pitch is indirectly specified via the Passages in 360 setting on the Basic
Settings tab for the domain.
This resulting time period is displayed as the Passing Period.
•
Automatic
When this option is selected, the time period is calculated automatically. The calculation uses the
information specified for each disturbance, and the blade pitch of the domain. Note that the blade
pitch of a domain is indirectly specified via the Passages in 360 setting on the Basic Settings tab
for the domain.
The time period is given a value such that, during one period, each disturbance undergoes an integer
number of cycles. This time period is displayed as the Passing Period.
The Min. Timesteps / Period is computed and displayed; it is the minimum number of time steps
required to resolve each disturbance cycle period into an integer number of time steps.
In a typical transient simulation, you can specify the time step size directly. However, when using a
Transient Blade Row model, the time step size is set indirectly.
The Time Steps settings control the size of a time step indirectly in one of two ways, depending on
the option you choose:
•
Number of Timesteps per Period
The time step size is computed by dividing the Passing Period by a number, Timesteps per
Period, that you specify.
•
Timestep Multiplier (available only when the Time Period option is set to Automatic)
The time step size is computed by dividing the Passing Period by the number of time steps per
period, where the latter is the product of Min. Timesteps / Period and Timestep Multiplier.
You must ensure that the number of time steps per period is sufficient to resolve each disturbance.
You must also ensure that the number of time steps per disturbance cycle period is an integer number.
When using the Fourier Transformation method, it is essential to use an integer number for reasons of
stability and accuracy. When using the Time Transformation method, the use of an integer number is
recommended and is important for accuracy in post-processing the results.
The Time Duration settings control the length of the simulation directly by controlling the number of
periods. This setting also indirectly controls the total number of time steps in the simulation.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
243
244
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 23: Mesh Adaption
Mesh Adaption in CFX is the process by which the mesh is selectively refined in areas that are affected
by the adaption criteria specified. This means that as the solution is calculated, the mesh can automatically be made finer or coarser in locations where solution variables change rapidly, in order to resolve
the features of the flow in these regions.
Each mesh element is given an Adaption Level. Each time the element is split into smaller elements,
the new elements are assigned an Adaption Level that is one greater than the element it was generated
from. The maximum number of Adaption Levels is controlled to prevent over-refinement.
In CFX, mesh adaption is available for single domain, steady-state problems; you cannot combine mesh
adaption with Domain Interfaces, combine it with Solid Domains, or use it for an ANSYS Multi-field
simulation. The Mesh Adaption process is performed by CFX-Solver. However, the parameters that
control the Adaption process are defined in CFX-Pre on the Mesh Adaption form.
This chapter describes:
•
Overview (p. 245)
•
Setting Up Mesh Adaption (p. 246)
•
The Details View for Mesh Adaption (p. 247)
•
Advanced Topic: Adaption with 2D Meshes (p. 250)
23.1. Overview
The following will take place when CFX-Solver is run (on steady-state problems). The process is shown
in the diagrammatic form below (Figure 23.1 (p. 246)).
1.
The CFX-Solver solves for solution variables using the mesh that is contained in the CFX-Solver input
file, or specified using an initial values file. The CFX-Solver uses Convergence Criteria that have been
specified on the Basic Settings tab of the Mesh Adaption form; the Convergence Criteria specified
on the Solver Control form is not used at this stage.
2.
A Mesh Adaption Step (one loop of the adapt-solve cycle) takes place. Using the solution calculated
in this first step, together with the Adaption Criteria specified on the Mesh Adaption Basic Settings
form, the mesh is refined in selected areas. For details, see Mesh Adaption in the CFX-Solver Theory
Guide.
3.
The CFX-Solver solves for solution variables using the mesh created by the Mesh Adaption step. The
CFX-Solver uses the Convergence Criteria specified on the Basic Settings tab of the Mesh Adaption
form; the Convergence Criteria specified on the Solver Control form is not used at this stage.
4.
Steps 2 and 3 are repeated until the Max. Num. Steps (specified on the Basic Settings of the Mesh
Adaption form) is reached.
5.
Finally, CFX-Solver solves for solution variables using the mesh that was created by the final Mesh
Adaption step. The Convergence Criteria used by the CFX-Solver at this stage are those specified on
the Solver Control form.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
245
Chapter 23: Mesh Adaption
Figure 23.1 Mesh Adaption Process
The Mesh Adaption step itself consists of the following:
1.
The Adaption Criteria are applied to each edge of each element in the mesh.
2.
Nodes are added to the existing mesh according to the Adaption Criteria. The number of nodes added
is dependent on the total number of nodes to be added and the node allocation parameter.
3.
The solution already calculated on the older mesh is linearly interpolated onto the new mesh.
If the CFX-Solver is being run in parallel, then each “Solve” step is preceded by a mesh partitioning
step.
Additional information on how elements are selected for adaption, how elements are divided, and the
limitations of mesh adaption in CFX is available in Mesh Adaption in the CFX-Solver Theory Guide.
23.2. Setting Up Mesh Adaption
To set up mesh adaption:
246
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Mesh Adaption
1.
Select Insert > Solver > Mesh Adaption.
The Mesh Adaption dialog box appears.
2.
Select or clear Activate Adaption.
If selected, Mesh Adaption performs when the solver is run.
3.
Under Region List, select the regions to adapt.
For details, see Region List (p. 248).
4.
Select or clear Save Intermediate Files.
For details, see Save Intermediate Files (p. 248).
5.
Specify the required Adaption Criteria.
For details, see Adaption Criteria (p. 248).
6.
Specify the required Adaption Method.
For details, see Adaption Method (p. 249).
7.
Specify Adaption Convergence Criteria.
For details, see Adaption Convergence Criteria (p. 249).
8.
Select Adaption Variables from the Variables List.
9.
Enter the Maximum Number of Adaption Steps (Max. Num. Steps ) allowed.
The default is 3. For details, see Max. Num. Steps (p. 248).
10. Select how many nodes should be present in the adapted mesh. Options are:
•
Multiple of Initial Mesh
•
Final Number of Nodes
For details, see Option (p. 249).
11. Select an option for Adaption Method > Option.
For details, see Adaption Method (p. 249).
12. Specify the Adaption Convergence Criteria to be used for each adaption step.
For details, see Adaption Convergence Criteria (p. 249).
This is different from the Convergence Criteria used to terminate the run, which is set in Solver
Controller. For details, see Basic Settings Tab (p. 199).
13. Switch to the Advanced Options tab or click OK to accept the mesh adaption settings. For details,
see Advanced Options Tab (p. 249).
23.3. The Details View for Mesh Adaption
The following tabs are presented on the details view of Mesh Adaption:
•
Basic Settings Tab (p. 248)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
247
Chapter 23: Mesh Adaption
•
Advanced Options Tab (p. 249)
23.3.1. Basic Settings Tab
The following sections describe the options available on the Basic Settings tab for Mesh Adaption.
23.3.1.1. Region List
Region List contains the names of all 3D Regions and Assemblies in the problem. Select any or all of
the 3D regions to be used for mesh adaption.
Note
Mesh adaption cannot be used in multidomain simulations or in cases with external solver
coupling. Mesh adaption also cannot be used for transient, mesh-motion, radiative-tracking,
or particle-transport cases.
23.3.1.2. Save Intermediate Files
If Save Intermediate Files is selected, an intermediate results file is saved immediately before each
mesh adaption step begins. At the end of the run, these intermediate files are stored in a subdirectory
with the same name as the run, in the directory that contains the CFX-Solver results file.
23.3.1.3. Adaption Criteria
For each adaption step, and for each mesh element, the adaption criteria are applied, and mesh elements
meeting the adaption criteria are refined. There are two methods of specifying how the adaption criteria
are specified. For details, see Adaption Method (p. 249).
23.3.1.3.1. Variables List
The Variables List is used to select the variables that make up part of the Adaption Criteria.
During the adaption process, if only one variable is selected, the value of the variable is observed for
each element defining the selected regions specified by the Region List. The maximum variation in
value of the variable along any edge of an element is used to decided whether the element is to be
modified. If multiple variables are selected, the maximum of variation of all the variables for a given
element is used to decide whether or not an element should be modified.
To save unnecessary processing, it is important to ensure that variables selected will vary during the
calculation. For instance, do not select Density as a variable for an incompressible flow calculation.
23.3.1.3.2. Max. Num. Steps
The number of steps that the adaption process performs is specified by Max. Num. Steps. It is recommended that you select a number between 1 and 5.
Note
If CFX-Solver runs on the CFX-Solver input file and finishes normally, this number of Adaption
Steps will take place. If CFX-Solver is stopped and then restarted from the results file produced,
only the remaining number of Adaption Steps will take place in the restarted run.
248
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Mesh Adaption
23.3.1.3.3. Option
The number of nodes in the final mesh generated by the adaption process is controlled by the value
selected in Option.
Select Final Number of Nodes, to specify the number of nodes in the final mesh, or Multiple of Initial
Mesh, which enables specification of the number of nodes in the final mesh as a multiple of the initial
mesh.
If Multiple of Initial Mesh is selected, it is also necessary to specify a Node Factor multiplier greater
than 1.2. If Final Number of Nodes is selected, then specify the number of Nodes in Adaption Mesh
that is no more than a factor of five greater than the number of nodes in the initial mesh.
Note
The final mesh will not contain exactly the number of nodes specified in either case. For
details, see Mesh Adaption in the CFX-Solver Theory Guide.
23.3.1.4. Adaption Method
The Adaption Method used by the adaption process to apply the Adaption Criteria is controlled by
the options specified in the Adaption Method section of the form.
23.3.1.4.1. Option
The Adaption Method is specified as either Solution Variation, or Solution Variation * Edge Length.
If Solution Variation * Edge Length is selected, the Adaption Criteria takes account of both the
variation of the solution variable over the edge of the element and the length of the edge. The result
of having applied the Adaption Criteria to each edge of an element is then multiplied by the length
of the edge. The maximum value of all the edges of the element is used to decide whether an element
is to be refined. This means that in areas of the flow where the solution variation is similar, adaption
will take place preferentially in regions where the mesh length scale is largest.
23.3.1.4.2. Minimum Edge Length
When Solution Variation is specified by Option, the Adaption Criteria is applied using only the maximum variation of a solution variable across any edge associated with an element. This option does not
use the length of the edge in the calculation. In this case, consider specifying a Minimum Edge Length
to avoid refining the mesh too far at a discontinuity in the solution. For details, see Mesh Adaption in
the CFX-Solver Theory Guide.
23.3.1.5. Adaption Convergence Criteria
The convergence criteria used to specify when the CFX-Solver stops running on the original and intermediate meshes is specified in the Adaption Convergence Criteria section of the form. The available
parameters are the same as those used to determine the final convergence of the solution. For details,
see Basic Settings Tab (p. 199).
23.3.2. Advanced Options Tab
It is possible to specify some further parameters to control the adaption process, these are specified
on the Advanced Options tab of the Mesh Adaption form.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
249
Chapter 23: Mesh Adaption
23.3.2.1. Node Alloc. Param.
Setting the node allocation parameter, Node Alloc. Param., controls how much the mesh is refined at
each adaption step. For some problems, it may be that it is better to refine a lot in the early steps, and
for others it may be more appropriate to refine more in the later steps.
Node Alloc. Param. is used as follows. On the nth adaption step, approximately Sn nodes are added
to the mesh, where
=
−
∑ − M is the maximum number of nodes that can be added to the original mesh calculated from having
applied the Adaption Criteria to the selected regions and c is the value of Node Alloc. Param.. For
details, see Adaption Criteria (p. 248).
When Node Alloc. Param. is set to 0, then the same number of nodes is added for each adaption step.
When Node Alloc. Param. is negative, more nodes are added in the later adaption steps. When it is
positive, more nodes are added in the earlier adaption steps. The table below shows the percentage
of nodes that will be added at each adaption step when Max. Num. Steps is set to a value of 3 and
different values of Node Alloc. Param. are specified.
Node Alloc. Param
Step
1
Step 2
Step
3
-2.0
7.14
28.57
64.28
-1.0
16.66
33.33
50.00
0.0
33.33
33.33
33.33
0.5
43.77
30.95
25.27
1.0
54.54
27.27
18.18
2.0
73.47
18.36
8.16
It is recommended that you set a value for Node Alloc. Param. in the range -2 to 2.
23.3.2.2. Number of Levels
The value of this parameter specifies the maximum number of times any element of the original mesh
can be subdivided. It must not be greater than Max. Num. Steps.
23.4. Advanced Topic: Adaption with 2D Meshes
2D Meshes are not supported in CFX. However, CFX can use 3D meshes that are one element thick.
This section outlines a workaround for such meshes when using mesh adaption.
CFX 2D meshes contain hexahedral, prismatic and potentially pyramidal and tetrahedral elements. In
the support of prismatic inflation in 3D meshes, special restrictions are applicable to the adaption of
prismatic elements. If adaption is applied to a 3D mesh that is one element thick, an error will result.
In order to work around this, set the environment variable CFX5_REFINER_NO_TRICOLUMNS to 1
before starting CFX-Pre. Note that any refinement that takes place will be 3D refinement that will introduce additional elements in the third dimension. This environment variable can also be used when the
250
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Advanced Topic: Adaption with 2D Meshes
input mesh has prismatic elements that have opposite triangular faces on the boundary. This can arise
if the mesh has been imported from a mesh generation tool other than CFX-Mesh.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
251
252
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 24: Expert Control Parameters
This chapter describes:
•
Modifying Expert Control Parameters (p. 253)
All geometry, domain, boundary condition, mesh, initial value and solver parameter information is
written to the CFX-Solver Input (.def) File.
The CFX-Solver input file contains the relevant information required by the CFX-Solver to conduct the
CFD simulation. This information mainly consists of numerical values that set up the simulation, as well
as controls for the CFX-Solver.
Many of these parameters are set in CFX-Pre. For example, on the Solver Control panel, you can set
the accuracy of the numerical discretization. Other settings, particularly those controlling the CFXSolver, cannot be set in the normal way through the CFX-Pre interface. These are called Expert Control
Parameters and have default values that do not require modification for the majority of CFD simulations.
For details, see When to Use Expert Control Parameters in the CFX-Solver Modeling Guide and CFXSolver Expert Control Parameters in the CFX-Solver Modeling Guide.
24.1. Modifying Expert Control Parameters
1.
Select Insert > Solver > Expert Parameter.
The Extra Parameters details view appears.
2.
Make changes to the appropriate sections on any of the following tabs: Discretization, Linear Solver,
I/O Control, Convergence Control, Physical Models, Particle Tracking, or Model Overrides.
Making changes requires selecting options and setting specific values. For parameters with a small
number of choices (such as logical parameters), select an option from the drop-down list. Other
parameters require data entry (such as real numbers).
For details on each of the parameters listed on these tabs, see CFX-Solver Expert Control Parameters
in the CFX-Solver Modeling Guide.
3.
Repeat the previous step as desired.
4.
Click OK.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
253
254
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 25: Coordinate Frames
By default, all quantities used in CFX-Pre are defined with reference to the global Cartesian coordinate
frame. In some cases, it is useful to use a different coordinate frame for specifying boundary conditions,
initial conditions, source components or spatially varying material properties. It is possible to specify
one or more local coordinate frame objects which can then be referred to. This chapter describes the
user interface for creating local coordinate frame objects. For details, see Coordinate Frames in the CFXSolver Modeling Guide.
Local Coordinate Frame objects may be defined in terms of Cartesian coordinates. Here, the numbers
1, 2, 3 are used to denote the Cartesian X, Y, Z axes.
This chapter describes:
25.1. Creating a New Coordinate Frame
25.2. Coordinate Frame Basic Settings Tab
25.1. Creating a New Coordinate Frame
1.
Select Insert > Coordinate Frame.
The Insert Coordinate Frame dialog box appears
2.
Set Name to a unique name for the coordinate frame.
Coord 0 cannot be used as a name as it is the default coordinate frame. For details, see Valid
Syntax for Named Objects (p. 55).
3.
Click OK.
The coordinate frame details view appears, with the Basic Settings tab visible.
4.
Specify the basic settings.
For details, see Coordinate Frame Basic Settings Tab (p. 255).
5.
Click OK.
An object named after the coordinate frame is created and listed in the tree view under Simulation.
25.2. Coordinate Frame Basic Settings Tab
The Basic Settings tab for a coordinate frame object contains settings that specify the coordinate frame.
It is accessible by creating a new coordinate frame or by editing a coordinate frame listed in the tree
view.
25.2.1. Coordinate Frame: Option
25.2.2. Coordinate Frame: Centroid
25.2.3. Coordinate Frame: Direction
25.2.4. Coord Frame Type
25.2.5. Reference Coord Frame
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
255
Chapter 25: Coordinate Frames
25.2.6. Origin
25.2.7. Z-Axis Point
25.2.8. X-Z Plane Point
25.2.9. Frame Motion Settings
25.2.10. Visibility Check Box
25.2.1. Coordinate Frame: Option
25.2.1.1. Point and Normal
This method can be used to make Cartesian coordinate frames. The origin of the coordinate frame is
set to the centroid of a specified 2D region (which is available only when a mesh exists). Axis 3 of the
coordinate frame is then computed as locally normal to the 2D region; its direction can be reversed if
not satisfactory (after examining the coordinate frame representation in the viewer). Optionally, Axis 1
may be given a prescribed orientation about Axis 3 by specifying a point that is interpreted as lying on
the 1-3 plane with a positive Axis 1 coordinate. If such a point is not specified explicitly, the global origin
is used. Axis 2 is found by the right-hand rule.
25.2.1.2. Axis Points
This method can be used to make Cartesian coordinate frames. The coordinate frame is created by
specifying three points. It is important to understand how these three points are used to create a coordinate frame. For details, see Coordinate Frame Details in the CFD-Post User's Guide.
25.2.2. Coordinate Frame: Centroid
25.2.2.1. Location
(applies only when Option is set to Point and Normal)
Select a 2D region or combination of 2D regions, the centroid of which will be used as the origin of
the coordinate frame.
Tip
Hold the Ctrl key when clicking to select multiple regions.
Tip
With Single Select
for selection.
selected, you may click locations in the viewer to make them available
25.2.2.2. Centroid Type
(applies only when Option is set to Point and Normal)
•
Absolute
The true centroid position is used. If the specified region is not planar, the absolute centroid may
not lie on the surface.
•
256
Nearest Point on Mesh
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Coordinate Frame Basic Settings Tab
The mesh node nearest to the true centroid is used.
25.2.3. Coordinate Frame: Direction
25.2.3.1. Invert Normal Axis Direction Check Box
(applies only when Option is set to Point and Normal)
This check box determines whether or not the direction of the Z-axis is reversed from that initially determined.
25.2.3.2. Point on Reference Plane 1-3 Check Box
(applies only when Option is set to Point and Normal)
This check box determines whether or not the theta=0 direction is defined explicitly by a point in the
1-3 plane. If selected, you must specify that point.
25.2.3.3. Point on Reference Plane 1-3 Check Box: Coordinate
Enter global Cartesian coordinates that define a point on the 1-3 plane of the coordinate frame. The
direction of this point from the nearest point on Axis 3 is the direction of Axis 1. Axis 1 corresponds
with the radial direction for theta=0.
Tip
With Single Select
responding points.
selected, you may click 2D locations in the viewer to select their cor-
25.2.4. Coord Frame Type
(applies only when Option is set to Axis Points)
Coordinates interpreted with reference to the coordinate frame will be interpreted as Cartesian. For
details, see Cartesian Coordinate Frames in the CFX-Solver Modeling Guide.
25.2.5. Reference Coord Frame
(applies only when Option is set to Axis Points)
Select an existing coordinate frame to use as a basis for interpreting the point data that defines the
present coordinate frame.
25.2.6. Origin
(applies only when Option is set to Axis Points)
In the reference Coordinate Frame, enter coordinates that define the origin of the present coordinate
frame.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
257
Chapter 25: Coordinate Frames
Tip
With Single Select
responding points.
selected, you may click 2D locations in the viewer to select their cor-
25.2.7. Z-Axis Point
(applies only when Option is set to Axis Points)
In the reference Coordinate Frame, enter coordinates that define a point on the positive side of the
Z-axis of the present Coordinate Frame.
Tip
With Single Select
selected, you may click locations in the viewer.
25.2.8. X-Z Plane Point
(applies only when Option is set to Axis Points)
In the reference Coordinate Frame, enter coordinates that define a point on the X-Z plane of the
present Coordinate Frame.
The direction of this point from the nearest point on the Z-axis is the direction of the X-axis.
Tip
With Single Select
selected, you may click locations in the viewer.
25.2.9. Frame Motion Settings
The options are:
•
Stationary
•
Rotating
You can specify a constant angular velocity for the coordinate frame by setting Option to Rotating
and specifying a (constant) value (which could be in the form of a CEL expression) for the Angular
Velocity. You will also have to specify a stationary axis about which the rotation occurs, using the
Axis Definition settings.
A boundary condition can use a rotating coordinate frame as its local frame of reference in order
to cause an applied profile (for example, a pressure profile) to move.
25.2.10. Visibility Check Box
This check box determines whether or not the graphics representation of the coordinate axis is displayed
in the viewer.
258
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 26: Materials and Reactions
The tree view contains a Materials object and a Reactions object, which contain all the currently
available materials and reactions.
A Material details view is available for editing the properties of new or existing fluids, solids, and mixtures. The new or modified materials can then be selected for use in your simulation or reaction definitions. For details, see Materials (p. 259).
A Reaction details view is available for editing the properties of new or existing reactions. For details,
see Reactions (p. 270).
Note
You can set only those material properties that will be used in the CFD model. For example,
you can set the buoyancy properties only if your model involves buoyant flow.
You can use CEL to define fluid property variation through an expression if it is required. For
example, you could define Dynamic Viscosity to be a function of Temperature.
26.1. Materials
The Material details view, accessible by editing a material from the tree view or by creating a new
material, is used to prepare materials for availability in a simulation.
The following topics will be discussed:
26.1.1. Library Materials
26.1.2. Material Details View: Common Settings
26.1.3. Material Details View: Pure Substance
26.1.4. Material Details View: Fixed Composition Mixture
26.1.5. Material Details View: Variable Composition Mixture
26.1.6. Material Details View: Homogeneous Binary Mixture
26.1.7. Material Details View: Reacting Mixture
26.1.8. Material Details View: Hydrocarbon Fuel
26.1.1. Library Materials
CFX-Pre provides an extensive list of library materials. Properties for these have already been defined
and are known to CFX-Pre. If you modify a library material during a simulation using the Material details
view, the modified definition is stored in the simulation file and is therefore local to your simulation.
On the Outline tab, right-click Materials and select Import Library Data to open the Select Library
Data to Import dialog box. From here, you can select a material to load.
. The dialog box will
If necessary, you can open the File to Import dialog box by clicking Browse
open with the default location: <CFXROOT>/etc/materials-extra/. This directory contains CCL
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
259
Chapter 26: Materials and Reactions
files that can be used to load additional materials into CFX-Pre (for example, Redlich Kwong, IAPWS, or
Interphase Mass Transfer materials).
If you want to use a material defined in one simulation in another simulation, the recommended
method is to use the Export and Import CCL features to load the material definition from a local file.
This is done by exporting CCL objects of type LIBRARY:LIBRARY/MATERIAL. For details, see Import
CCL Command (p. 35) and Export CCL Command (p. 36).
26.1.2. Material Details View: Common Settings
26.1.2.1. Option
Any material can consist of one or more materials. If a material contains only a single pure species, then
it is known as a pure substance. If it contains more than one species, then it is known as a mixture. The
materials are assumed to be mixed at the molecular level in the mixture.
The type of material is set using the following options:
•
The Pure Substance option should be used to create a fluid whose properties, such as viscosity,
density, or molar mass, are known. All existing and newly created pure substances appear in the materials list and you can then create mixtures from them. For details, see Material Details View: Pure Substance (p. 263).
•
The Fixed Composition Mixture option should be used to create a mixture with fixed mass
fractions of each material. The mass fraction of each material is specified and is not allowed to change
during the course of the simulation in space or time. For details, see Material Details View: Fixed Composition Mixture (p. 266).
•
The Variable Composition Mixture option should be used to create a mixture whose mass
fractions are allowed to change during the course of a simulation in space and time. The mass fraction
of each material is not specified when defining the fluid. You can use a fixed composition mixture as a
material in a variable composition mixture.
For details, see Material Details View: Variable Composition Mixture (p. 267).
•
The Homogeneous Binary Mixture option applies to equilibrium phase change calculations. For
details, see Material Details View: Homogeneous Binary Mixture (p. 267).
•
The Reacting Mixture option is used for a chemical reaction, such as combustion.
For details, see Material Details View: Reacting Mixture (p. 268).
•
The Hydrocarbon Fuel option. For details, see Material Details View: Hydrocarbon Fuel (p. 269).
26.1.2.2. Material Group
The Material Group filter is used to group materials by type, as well as restrict what materials can be
mixed when the physical models include reactions or phase change. A material can be a member of
more than one material group if it has a consistent set of properties. Material Group will always be
set to at least one of the following:
26.1.2.2.1. User
Any user-defined materials, not assigned to one of the other groups, are shown in or can be added to
this group. For example, materials loaded from a previous CFX-Pre simulation are shown in this group.
260
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Materials
26.1.2.2.2. Air Data
This group contains Ideal Gas and constant property air. Constant properties are for dry air at both 0
[C], 1 [atm] (STP) and 25 [C], 1 [atm].
26.1.2.2.3. CHT Solids
Contains solid substances that can be used for solid domains when performing conjugate heat transfer
modeling.
26.1.2.2.4. Calorically Perfect Ideal Gases
Contains gases that obey the Ideal Gas Law.
26.1.2.2.5. Constant Property Gases / Liquids
These groups contain gas and liquid substances with constant properties.
The gas properties are calculated at STP (0 [C] and 1 [atm]). Gas materials in this group can be combined
with NASA SP-273 materials for use in combustion modeling simulations.
26.1.2.2.6. Dry/Wet Redlich Kwong
No materials appear in this group by default, they must be loaded from a pre-supplied materials file.
All materials in this group use the built-in Redlich-Kwong equation of state and are suitable for performing
equilibrium, homogeneous, phase change modeling.
For any given pure substance, there are three different materials. There is a material with a RK tag, used
for dry vapor calculations, and three materials with RKv, RKl and RKlv suffixes, which are used for
equilibrium phase change (wet vapor) calculations.
26.1.2.2.7. Dry/Wet Redlich Kwong RGP
No materials appear in this group by default, they must also be loaded from a pre-supplied materials
file. All materials in this group use the Redlich-Kwong equation of state with properties specified in a
TASCflow RGP file. These materials are suitable for performing equilibrium, homogeneous, phase change
modeling.
Like the built-in Redlich Kwong group, for any given pure substance there are three different materials.
There is a material with a RK tag, used for dry vapor calculations, and three materials with RKv, RKl
and RKlv suffixes, which are used for equilibrium phase change (wet vapor) calculations.
26.1.2.2.8. Dry/Wet Peng Robinson RGP
No materials appear in this group by default, they must also be loaded from a pre-supplied materials
file. All materials in this group use the Redlich-Kwong equation of state with properties specified in a
TASCflow RGP file. These materials are suitable for performing equilibrium, homogeneous, phase change
modeling.
Like the built-in Redlich Kwong group, for any given pure substance there are three different materials.
There is a material with a RK tag, used for dry vapor calculations, and three materials with RKv, RKl
and RKlv suffixes, which are used for equilibrium phase change (wet vapor) calculations.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
261
Chapter 26: Materials and Reactions
26.1.2.2.9. Dry/Wet Soave Redlich Kwong RGP
No materials appear in this group by default, they must also be loaded from a pre-supplied materials
file. All materials in this group use the Redlich-Kwong equation of state with properties specified in a
TASCflow RGP file. These materials are suitable for performing equilibrium, homogeneous, phase change
modeling.
Like the built-in Redlich Kwong group, for any given pure substance there are three different materials.
There is a material with a RK tag, used for dry vapor calculations, and three materials with RKv, RKl
and RKlv suffixes, which are used for equilibrium phase change (wet vapor) calculations.
26.1.2.2.10. Dry/Wet Steam
No materials appear in this group by default, they must also be loaded from a pre-supplied materials
file. Materials in this group use the IAPWS equation of state. Again, the materials are suitable for either
dry or wet steam calculations.
26.1.2.2.11. Gas Phase Combustion
Contains materials that can be used for gas phase combustion. All materials in this group use the Ideal
Gas equation of state. The specific heat capacity, enthalpy and entropy for each of the materials are
specified using the NASA SP-273 format. For details, see NASA Format in the CFX-Solver Modeling Guide.
26.1.2.2.12. Interphase Mass Transfer
This group contains materials that can be used for Eulerian or Lagrangian interphase mass transfer. This
group currently contains a number of materials that have liquid or gas reference states, which are
consistent for performing phase change calculations. The gas phases use the ideal gas equation of state
and temperature dependent specific heat capacity. The associated liquid phases use constant properties.
26.1.2.2.13. Particle Solids
Contains a list of solids that can be used in Particle Tracking calculations.
26.1.2.2.14. Soot
This group contains solid substances that can be used when performing soot calculations.
26.1.2.2.15. Water Data
This group contains liquid and vapor water materials with constant properties. The materials in this
group can be combined with NASA SP-273 materials for use in combustion modeling simulations.
26.1.2.3. Material Description
This parameter can be toggled on to view a detailed description of the substance. Click Edit the Material
Description
to edit the description (to a maximum of 120 alphanumeric characters).
26.1.2.4. Thermodynamic State
This parameter sets the state of a substance to solid, liquid or gas. There are certain limitations imposed
by selecting a particular state. For example, a solid must always have at least density, specific heat capacity and thermal conductivity specified.
262
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Materials
26.1.2.5. Coord Frame
For material properties that are set using expressions containing X, Y, or Z, you may want to supply a
custom coordinate frame as the basis for evaluation of such properties. For details, see Coord
Frame (p. 263), Coordinate Frames (p. 255), and Coordinate Frames in the CFX-Solver Modeling Guide.
26.1.3. Material Details View: Pure Substance
The following topics will be discussed:
•
Basic Settings Tab (p. 263)
•
Material Properties Tab (p. 263)
26.1.3.1. Basic Settings Tab
The Basic Settings tab is used to set the type of material, its state, an optional description and an optional coordinate frame.
1.
Set the Material Group.
For details, see Material Group (p. 260).
2.
The Material Description field is optional.
For details, see Material Description (p. 262).
3.
Select the Thermodynamic State.
For details, see Thermodynamic State (p. 262).
4.
Optionally set a custom coordinate frame for any material properties that depend on expressions in
X, Y, or Z.
For details, see Coord Frame (p. 263), Coordinate Frames (p. 255), and Coordinate Frames in the CFXSolver Modeling Guide.
26.1.3.2. Material Properties Tab
There are two main categories specifying properties of a pure substance: General Material and
Table. A General Material can have its thermodynamic, transport and radiation properties defined
in the most general manner using any of the built-in flow solver models, constants, or CEL expressions.
A table material uses a TASCflow RGP file to look up the required values. For details, see Table (p. 265).
26.1.3.2.1. General Material
General Materials can have their Equation of State set to the following options:
•
Equation of State - Value (p. 264).
•
Equation of State - Ideal Gas (p. 264).
•
Equation of State - Real Gas (p. 264).
For details on equations of state, see Equation of State in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
263
Chapter 26: Materials and Reactions
26.1.3.2.1.1. Equation of State - Value
The following tab appears when Equation of State is set to Value. Value uses whichever model for
density that is supplied by the user. For example, the equation of state model could be a constant or
a CEL expression.
•
Equation of State > Option. For details, see Option in the CFX-Solver Modeling Guide.
•
Specify the Density and Molar Mass. An expression can be used for Density that depends on temperature and/or pressure. In this case, the CFX-Solver may build property tables in order to calculate enthalpy
and entropy. If you use this option, check the table generation settings.
Additional information on Material Properties is available in:
•
Specific Heat Capacity in the CFX-Solver Modeling Guide
•
Transport Properties in the CFX-Solver Modeling Guide
•
Radiation Properties in the CFX-Solver Modeling Guide
•
Buoyancy Properties in the CFX-Solver Modeling Guide
•
Electromagnetic Properties in the CFX-Solver Modeling Guide.
26.1.3.2.1.2. Equation of State - Ideal Gas
•
If you set the specific heat capacity using a CEL expression, the solver will build tables for enthalpy and
entropy. If you use this option, check the table generation settings.
•
For an ideal gas, specify the Molar Mass. For details, see Molar Mass in the CFX-Solver Modeling Guide.
Additional information on ideal gas is available in:
•
Ideal Gas in the CFX-Solver Modeling Guide
•
Reference State Properties in the CFX-Solver Modeling Guide
•
Transport Properties in the CFX-Solver Modeling Guide.
26.1.3.2.1.3. Equation of State - Real Gas
The Real Gas option can be specified to model non-ideal gases and some liquid phase properties.
Set Model to one of the following:
•
Aungier Redlich Kwong (the default model)
•
Peng Robinson
•
Soave Redlich Kwong
•
Standard Redlich Kwong.
To load the Real Gas materials into CFX-Pre:
1.
On the Outline tab, right-click Materials and select Import Library Data.
2.
and open the MATERIALSIn the Select Library Data to Import dialog box, click Browse
redkw.ccl, MATERIALS-sredkw.ccl, or MATERIALS-pengrob.ccl file, which contain predefined real gas materials model.
3.
Select the group of materials to load and click OK.
264
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Materials
4.
Complete all of the data fields on the Materials Properties tab to use a Real Gas equation of state,
then click OK.
Additional information on Real Gas models is available in:
•
Real Gas in the CFX-Solver Modeling Guide
•
Specific Heat Capacity in the CFX-Solver Modeling Guide
•
Transport Properties in the CFX-Solver Modeling Guide.
•
Real Gas Properties in the CFX-Solver Theory Guide
26.1.3.2.2. Table
Table uses a CFX-TASCflow real gas property (RGP) file to load real fluid property data (see Real Fluid
Properties in the CFX-Solver Modeling Guide). You can load all of the RGP files that are supplied with
CFX quickly by following the instructions given in Loading an .rgp file in the CFX-Solver Modeling Guide.
When defining materials that use data in tables not supplied with CFX, the definition is carried out
separately by specifying the filename and component name for each material in turn. When Table is
selected, the following form appears:
TASCflow RGP file Table Format is the only type supported for CFX.
beside Table Name to browse to the file containing the Real Gas Property Table data.
1.
Click Browse
2.
Enter the Component Name (as an RGP file can contain many components).
The component name corresponds to the name of a component in an RGP file. You may need to
open the RGP file in a text editor to discover the exact name of the component you want to select.
For details, see Detailed .rgp File Format in the CFX-Solver Modeling Guide.
26.1.3.2.3. Table Generation
For some equation of state and specific heat capacity settings (such as Redlich Kwong, IAPWS, and
general materials having variable density and specific heat set with CEL expressions), the CFX-Solver
builds internal property tables for efficient property evaluation. The most commonly required table is
enthalpy as a function of temperature and possibly pressure. This table is built if the specific heat capacity
is a function of temperature, and, possibly pressure. Entropy tables are also used to convert static and
total pressure (or vice versa). For example, at a boundary condition you may specify the total pressure
and the flow solver will use entropy tables to calculate the static pressure. When using CEL expressions
for density and specific heat capacity the solver uses an adaptive algorithm to control the generation
of the tables. In some cases, it may be necessary to alter some table generation details, as described
by the following parameters:
26.1.3.2.3.1. Minimum and Maximum Temperature
These correspond to the lower and upper temperature bounds of the table. The selected values should
exceed the expected temperature range somewhat, but to keep the size of the table from becoming
too big, it should not exceed the expected range by a factor much greater than 2.
26.1.3.2.3.2. Minimum and Maximum Absolute Pressure
These correspond to the lower and upper absolute pressure bounds of the table. As with the temperature
bounds, the selected values should exceed the expected absolute pressure range, but not by too much.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
265
Chapter 26: Materials and Reactions
26.1.3.2.3.3. Error Tolerance
The table generation algorithm used by the solver is adaptive, and may cluster values where needed
to resolve nonlinearities in the property definitions. The table generation is required to satisfy an error
tolerance, defined as the relative error between the interpolation error and the exact value. The default
tolerance (0.01 for enthalpy and 0.03 for entropy) is usually adequate.
26.1.3.2.3.4. Maximum Points
This parameter specifies the maximum number of points (values) for each table dimension. Fewer points
may be required if the error criterion is met sooner. The default value of 100 is usually adequate.
Note
If the error tolerance cannot be met with the specified maximum number of points, the CFXSolver will revert to a uniform table with a resolution set to the maximum number of points.
26.1.3.2.3.5. Pressure/Temperature Extrapolation
This controls the solver behavior when evaluating properties at temperatures or pressures beyond the
table range. If extrapolation is activated, the property will be extrapolated based on its slope at the
table boundary; otherwise, the value at the table boundary will be used. In either case, a message is
written to the output file that an out-of-bounds has occurred. If this happens, you should consider increasing the table range accordingly.
26.1.4. Material Details View: Fixed Composition Mixture
This panel describes the Material details view when creating a fixed composition mixture. Fixed composition mixtures can consist of pure substances only and not other fixed composition mixtures. You
can include any combination of materials in a fixed composition mixture. To combine materials from
different material groups, however, you must first select the Material Groups that contain those materials. For example, to select Air at 25 C and Water at 25 C, you would first need to select the
groups Air Data and Water Data.
For details, see Multicomponent Flow in the CFX-Solver Modeling Guide.
26.1.4.1. Basic Settings Tab
1.
Select the Material Group(s) that contain the required materials.
2.
Use Materials List to add new materials to the mixture.
3.
The Material Description field is optional.
For details, see Material Description (p. 262).
4.
Select the Thermodynamic State.
For details, see Thermodynamic State (p. 262).
5.
Optionally set a custom coordinate frame for any material properties that depend on expressions in
X, Y or Z.
For details, see Coord Frame (p. 263), Coordinate Frames (p. 255), and Coordinate Frames in the CFXSolver Modeling Guide.
266
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Materials
6.
Select a material, from the Child Materials list box.
7.
Enter the fixed Mass Fraction of the material within the mixture.
The sum of the mass fractions for all the materials in a mixture must be 1.
26.1.4.2. Mixture Properties Tab
Mixture Properties can be used to explicitly set values when the Ideal Mixture model produces unsatisfactory results. The same options apply for fixed composition mixtures as for variable composition
mixtures. For details, see Mixture Properties Tab (p. 267).
26.1.5. Material Details View: Variable Composition Mixture
This panel describes the Material details view when creating a variable composition mixture. Components
of a variable composition mixture can be pure substances and fixed composition mixtures. For details,
see Multicomponent Flow in the CFX-Solver Modeling Guide.
26.1.5.1. Basic Settings Tab
1.
Select the Material Group(s) that contain the required materials.
2.
Use Materials List to add new materials to the mixture.
3.
The Material Description field is optional.
For details, see Material Description (p. 262).
4.
Select the Thermodynamic State.
For details, see Thermodynamic State (p. 262).
5.
Optionally set a custom coordinate frame for any material properties that depend on expressions in
X, Y or Z.
For details, see Coord Frame (p. 263), Coordinate Frames (p. 255), and Coordinate Frames in the CFXSolver Modeling Guide.
26.1.5.2. Mixture Properties Tab
When you create a fixed composition, variable composition, or a reacting mixture, then the fluid properties are determined by mass averaging the properties of the component materials. In some cases, the
ideal mixture rule used by the CFX-Solver may not be representative of the mixture properties. You can
override the individual thermodynamic and transport properties by enabling the appropriate toggles
and directly specifying the mixture properties. For details, see Mixture Properties (Fixed and Variable)
in the CFX-Solver Modeling Guide. For additional information on options for Specific Heat Capacity, see
Specific Heat Capacity in the CFX-Solver Modeling Guide. For details on modeling the reacting mixtures,
see Using Combustion Models in the CFX-Solver Modeling Guide.
26.1.6. Material Details View: Homogeneous Binary Mixture
Homogeneous binary mixtures are used to define the phase boundary between two chemically equivalent
materials in different thermodynamic states. For example, you could define the vapor pressure curve
between water and steam. The vapor pressure curve is used by the flow solver to determine the saturation properties of the two materials. A homogeneous binary mixture is required for running the Equi-
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
267
Chapter 26: Materials and Reactions
librium phase change model. Additionally, it can be used with the Eulerian multiphase thermal phase
change model or the Lagrangian particle tracking evaporation model.
The Basic Settings tab is used to specify the two materials that form the mixture. On the Saturation
Properties tab, the saturation properties can be specified.
26.1.6.1. Basic Settings Tab
1.
Select the Material Group(s).
2.
Select the two constituent materials for the binary mixture.
3.
The Material Description field is optional.
For details, see Material Description (p. 262).
26.1.6.2. Saturation Properties Tab
26.1.6.2.1. General
The General option can be used to specify the saturation temperature or Antoine coefficients for
materials that do not use a table or Redlich Kwong equation of state. If you set Pressure > Option to
Antoine Equation option, then the flow solver automatically calculates saturation temperature.
For details, see Antoine Equation in the CFX-Solver Modeling Guide. If you set Pressure > Option to
Value, you must specify the saturation pressure and the corresponding saturation temperature. For
details, see Using a General Setup in the CFX-Solver Modeling Guide.
26.1.6.2.2. Table
Files of type (*.rgp) are filtered from the list of files in the current directory.
26.1.6.2.3. Real Gas
When Real Gas is chosen, the saturation properties are calculated using the material properties
specified for the constituent components, and there is no need to set any values. As a consequence,
the material properties for components in the mixture must all use the same Real Gas equation of state.
For details, see Using a Real Gas Equation of State in the CFX-Solver Modeling Guide.
26.1.6.2.4. Table Generation
For details, see Table Generation (p. 265).
26.1.7. Material Details View: Reacting Mixture
The following topics will be discussed:
•
Basic Settings Tab (p. 268)
•
Mixture Properties Tab (p. 269)
26.1.7.1. Basic Settings Tab
A reacting mixture contains at least one reaction. For details, see Reactions (p. 270). The details for each
of the components are set under Component Details on the Fluid Models tab when defining your
domain. For details, see Fluid Models Tab (p. 113).
268
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Materials
1.
Select the Material Group types.
2.
Select the reactions from the Reactions List.
3.
The Material Description field is optional.
For details, see Material Description (p. 262).
4.
Select the Thermodynamic State.
For details, see Thermodynamic State (p. 262).
5.
Optionally set a custom coordinate frame for any material properties that depend on expressions in
X, Y, or Z.
For details, see Coord Frame (p. 263), Coordinate Frames (p. 255), and Coordinate Frames in the CFXSolver Modeling Guide.
6.
From Additional Materials List, select any additional inert materials (which do not take part in any
reaction).
26.1.7.2. Mixture Properties Tab
Mixture properties for reacting mixtures are the same as for fixed and variable composition mixtures.
For details, see Mixture Properties Tab (p. 267).
26.1.8. Material Details View: Hydrocarbon Fuel
The following topics will be discussed:
•
Basic Settings Tab (p. 269)
•
Proximate/ Ultimate Analysis Tab (p. 269)
•
Mixture Materials Tab (p. 269)
More information about hydrocarbon fuel models is available in Hydrocarbon Fuel Model Setup in the
CFX-Solver Modeling Guide and in Hydrocarbon Fuel Analysis Model in the CFX-Solver Theory Guide.
26.1.8.1. Basic Settings Tab
This tab is identical to the Basic Settings tab for pure substances. For details, see Basic Settings Tab (p. 263).
26.1.8.2. Proximate/ Ultimate Analysis Tab
For details, see Hydrocarbon Fuel Analysis Model in the CFX-Solver Theory Guide.
26.1.8.3. Mixture Materials Tab
The material components in the model need to be mapped to solver alias names. For example, carbon
dioxide could be represented in the solver by CO2, Carbon Dioxide CO2, CO2 modified, and
so on.
Particle Mixture defines the components of the hydrocarbon fuel particles. The names for the ash,
char and raw combustible component materials must be given.
Gas Mixture is for identifying the components of the gas-phase reacting mixture. Two options are
available:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
269
Chapter 26: Materials and Reactions
•
Mixture asks for the name of the associated gas-phase material (reacting mixture) and provides
parameters to identify the components of the gas phase, which are relevant for the hydrocarbon fuel
model.
•
Mixture with HCN NO additionally enables entering the names for the gas components involved
in the fuel-nitrogen model.
Note that here the components of the gas phase are identified only for the hydrocarbon fuel model.
The reacting mixture material still must be created with all its components in the same way as for
gaseous combustion. It may have additional components in addition to those identified here.
Binary Mixture is for defining the homogeneous binary mixture material, which describes the heat
transfer between the particle and the fluid mixture. For the two materials in the binary mixture you
should specify the raw combustible material for the particle and the volatiles fuel for the gas phase.
26.2. Reactions
The Reaction details view, accessible by editing a reaction from the tree view or by creating a new reaction, is used to prepare reactions for availability in a simulation.
Once a reaction is created, it is available for inclusion in a fluid that is a reacting mixture or a variable
composition mixture. For details, see:
•
Material Details View: Reacting Mixture (p. 268)
•
Material Details View: Variable Composition Mixture (p. 267).
26.2.1. Basic Settings Tab
Four types of reactions can be created on the Basic Settings tab:
•
Single Step (p. 270)
•
Multiple Step (p. 271)
•
Flamelet Library (p. 272)
•
Multiphase (p. 272)
26.2.2. Single Step
This option displays three other tabs in addition to Basic Settings. One of them is a Reactants tab,
displaying a list of reactants and specifying the ratio with which they react together and the order of
the reaction. A list of products is also set on the Products tab and includes the ratio with which they
are produced. Reaction Rates has optional forward and backward reaction rates and third body terms
can be applied.
26.2.2.1. Single Step: Basic Settings
1.
Optionally, select Reaction Description to enter a description for the reaction (to a maximum of 120
alphanumeric characters).
2.
Optionally, specify any additional materials for this reaction using the Additional Materials List.
3.
Optionally, select Reaction or Combustion to set a reaction or combustion model.
Any settings specified here will override the choice of models selected on the Fluid Models tab
of the domains form (unless the choice of models on the Fluid Models form is set to None).
270
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reactions
This is implemented to allow reaction-step specific combustion modeling for multi-step reactions. For
details, see Reaction-Step Specific Combustion Model Control in the CFX-Solver Modeling Guide.
26.2.2.2. Single Step: Reactants
For details, see Multiphase: Reactants (p. 272).
1.
Option assumes the value Child Materials when creating a reaction involving one phase.
2.
Choose the reactant(s) to add from the Materials List drop-down.
3.
Enter the Stoichiometric Coefficient for the each of the selected components.
4.
Optionally, specify a reaction order.
If the reaction order is not entered, it will default to the same value as the stoichiometric coefficient.
26.2.2.3. Single Step: Products
The Products tab is identical to the Reactants tab, with the only difference being that the settings
here apply to the products instead of the reactants.
26.2.2.4. Single Step: Reaction Rates
1.
For each of Forward Reaction Rate and Backward Reaction Rate, Option defines the reaction rate
dependency. Select from:
•
Arrhenius in the CFX-Solver Modeling Guide
•
Arrhenius with Temperature PDF in the CFX-Solver Modeling Guide
•
Expression in the CFX-Solver Modeling Guide
2.
The Pre Exponential Factor and Temperature Exponent are required elements for the Arrhenius
reaction type.
3.
The temperature limit list (Lower Temperature and Upper Temperature) is required for the Arrhenius with Temperature PDF reaction type.
4.
Reaction Activation enables Activation Temperature or Activation Energy to be set.
5.
Some reactions require a Third Body Term to proceed.
For details, see Third Body Terms in the CFX-Solver Theory Guide.
6.
You can define a reaction in terms of a dependency, equilibrium or an expression.
For details, see Reaction Rate Types in the CFX-Solver Modeling Guide.
26.2.3. Multiple Step
A list of Single Step reactions is required to define a Multi Step reaction.
1.
Set Option to Multi Step.
Hold the Ctrl key to select multiple reactions from the list.
Alternatively, click Select from a second list
2.
to open the Materials List list box.
Optionally, select Reaction Description to enter a description for the reaction.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
271
Chapter 26: Materials and Reactions
26.2.4. Flamelet Library
A flamelet library is imported with optional customization of the Laminar Burning Velocity.
1.
Set Option to Flamelet Library.
2.
Click Browse
to browse to the flamelet library file. The file that contains your flamelet library should
be selected. Flamelet libraries can be created by library generation software, such as CFX-RIF. For details,
see CFX-RIF in the CFX-Solver Modeling Guide.
3.
Optionally, select Reaction Description to enter a description for the reaction.
4.
Select Laminar Burning Velocity to specify an expression for the laminar flame speed definition.
When using a flamelet library, the definition for the library is specified in the Reaction details view. The
name, library file and, optionally, laminar flame speed definition is specified. The reaction can then be
used in a fluid that is a variable composition mixture. For details, see Material Details View: Variable
Composition Mixture (p. 267). and Laminar Flamelet with PDF Model in the CFX-Solver Modeling Guide.
26.2.5. Multiphase
This option is used to create reactions between more than one phase. For details, see Reaction Models
in the CFX-Solver Modeling Guide.
26.2.5.1. Multiphase: Basic Settings
The setup of multiphase reactions is carried out by selecting the reaction Option to Multiphase. For
details, see Multiphase Reactions and Combustion in the CFX-Solver Modeling Guide.
1.
For multiphase reactions the only option available for the Material Amount Option is Mass Coefficient.
2.
Optionally, select Reaction Description to enter a description for the reaction.
26.2.5.2. Multiphase: Reactants
Multiphase reactions are specified in terms of Parent Materials (the phase containing a reacting
material), and Child Materials (the reacting materials themselves).
The Parent Materials List contains the phases from which reacting materials are selected.
1.
For the currently selected parent material, (such as Coal), select the reactant materials from that phase
from the materials list (for example, Coal > Materials List).
If a participating phase is a pure substance, it should be selected as both a parent and child material.
2.
For each child material, enter a mass coefficient.
3.
Reaction Order is only required for reactions of type Mass Arrhenius.
If unset, it defaults to 1.
26.2.5.3. Multiphase: Products
The setup on the Products tab is identical to the Reactants tab. For details, see Multiphase: Reactants (p. 272).
272
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reactions
26.2.5.4. Multiphase: Multiphase Reactions
The Multiphase Reaction Rate > Option can be one of:
•
Mass Arrhenius in the CFX-Solver Modeling Guide
•
Gibb Char Oxidation Model in the CFX-Solver Modeling Guide
•
Field Char Oxidation Model in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
273
274
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 27: Additional Variables
Additional Variables are non-reacting scalar components that can be transported through the flow.
Modeling information for Additional Variables is available:
•
Additional Variables in the CFX-Solver Modeling Guide
•
Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide
Implementation information for Additional Variables in multiphase flow is available:
•
Additional Variables in the CFX-Solver Theory Guide
•
Additional Variables in Multiphase Flow in the CFX-Solver Theory Guide
This chapter describes the procedure for creating an Additional Variable and the user interfaces used
to define and apply Additional Variables:
27.1. User Interface
27.2. Creating an Additional Variable
27.1. User Interface
The following topics are discussed:
•
Insert Additional Variable Dialog Box (p. 275)
•
Basic Settings Tab for Additional Variable Objects (p. 275)
•
Fluid Models and Fluid Specific Models Tabs for Domain Objects (p. 276)
•
Boundary Details and Fluid Values Tabs for Boundary Condition Objects (p. 279)
27.1.1. Insert Additional Variable Dialog Box
The Insert Additional Variable dialog box is used to initiate the creation of a new Additional Variable.
It is accessible by clicking the Additional Variable icon , or by selecting Insert > Expressions, Functions
and Variables > Additional Variable.
27.1.2. Basic Settings Tab for Additional Variable Objects
The Basic Settings tab is used to define the fundamental properties of an Additional Variable. It is accessible by creating a new Additional Variable or by editing an Additional Variable listed in the tree
view.
27.1.2.1. Variable Type
•
Specific
The Additional Variable is solved on a per-unit-mass basis. For details, see Volumetric and Specific
Additional Variable in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
275
Chapter 27: Additional Variables
•
Volumetric
The Additional Variable is solved on a per-unit-volume basis. For details, see Volumetric and Specific Additional Variable in the CFX-Solver Modeling Guide.
•
Unspecified
The Additional Variable is defined in terms of an algebraic expression using CEL. For details, see
Unspecified Additional Variables in the CFX-Solver Modeling Guide.
27.1.2.2. Units
Specify the units that describe the Additional Variable. For details, see Additional Variables in the CFXSolver Modeling Guide.
27.1.2.3. Tensor Type
The Additional Variable's Tensor Type can be set to Scalar or Vector. If an Additional Variable is
defined as type Vector, the components of a vector algebraic equation can be defined at the domain
level.
Vector Additional Variables cannot be directly referenced in CEL expressions. The syntax for referencing
a component of a vector Additional Variable is as follows:
<Component Name>.<Additional Variable Name>_x
27.1.3. Fluid Models and Fluid Specific Models Tabs for Domain Objects
The settings for Additional Variables on the Fluid Models tab are used to enable Additional Variables
in the domain. For multiphase simulations, settings for unspecified and volumetric Additional Variables
are available only on the Fluid Specific Models tab. For specific Additional Variables homogeneous
transport equations can be set on the Fluid Models tab or on a per-fluid basis on the Fluid Specific
Models tab if the Additional Variable has been set to Fluid Dependent on the Fluid Models tab.
27.1.3.1. Additional Variable Details: List Box
This list box is used to select an Additional Variable in order to set the details of its application to the
domain.
27.1.3.2. Additional Variable Details: [Additional Variable Name] Check Box
This check box determines whether or not the Additional Variable is to be modeled in the domain.
27.1.3.2.1. Option
27.1.3.2.1.1. Transport Equation
The transport of the Additional Variable of type Volumetric is modeled by a transport equation. For
details, see Additional Variables in the CFX-Solver Theory Guide.
27.1.3.2.1.2. Diffusive Transport Equation
The transport of the Additional Variable is modeled by a transport equation. The advection term is
dropped from the transport equation. For details, see Additional Variables in the CFX-Solver Theory Guide.
276
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
27.1.3.2.1.3. Homogeneous Transport Equation
The transport of the Additional Variable is modeled by a transport equation. This option is available
only on the Fluid Models tab and only for multiphase flows (that is, only for homogeneous applications).
For details, see:
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Theory Guide.
27.1.3.2.1.4. Homogeneous Diffusive Transport Equation
The transport of the Additional Variable is modeled by a transport equation. The advection term is
dropped from the transport equation. This option is available only on the Fluid Models tab and only
for multiphase flows (that is, only for homogeneous applications). For details, see:
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Theory Guide.
27.1.3.2.1.5. Poisson Equation
The transport of the Additional Variable is modeled by a transport equation. The transient and advection
terms are dropped from the transport equation. For details, see Additional Variables in the CFX-Solver
Theory Guide.
27.1.3.2.1.6. Homogeneous Poisson Equation
The transport of the Additional Variable is modeled by a transport equation. The transient and advection
terms are dropped from the transport equation. This option is available only on the Fluid Models tab
and only for multiphase flows (that is, only for homogeneous applications). For details, see:
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Modeling Guide
•
Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver Theory Guide.
27.1.3.2.1.7. Fluid Dependent
When the Fluid Dependent option is selected, the Additional Variable model details can be set for
each fluid on the Fluid Specific Models tab.
27.1.3.2.1.8. Algebraic Equation
A given quantity or CEL expression specifies the value of the Additional Variable throughout the domain.
Application of this option is, in the context of the fluids to which the Additional Variable is applied, effectively the same as setting the Additional Variable type to Unspecified.
27.1.3.2.1.9. Vector Algebraic Equation
A total of three given quantities, CEL expressions, or both, specifies the vector value of the Additional
Variable throughout the domain. Application of this option is, in the context of the fluids to which the
Additional Variable is applied, effectively the same as setting the Additional Variable type to Unspecified.
27.1.3.2.2. Value
(applies only when Additional Variable Details: [Additional Variable name] Check Box: Option is
set to Algebraic Equation)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
277
Chapter 27: Additional Variables
Enter a numerical quantity or CEL expression that specifies the value of the Additional Variable
throughout the domain.
27.1.3.2.3. Kinematic Diffusivity Check Box
(applies only when Additional Variable Details: [Additional Variable name] Check Box: Option is
set to Transport Equation, Diffusive Transport Equation, or Poisson Equation)
When running a Transport Equation Additional Variable, this check box determines whether the molecular diffusion term is added to the transport equation for the Additional Variable. For turbulent flow,
the turbulent diffusion term (which is a consequence of averaging the advection term) is automatically
included. Setting the kinematic diffusivity to zero includes the turbulent diffusion term only.
You must select this check box when using the Poisson equation or diffusive transport equation. If you
do not, a blue warning message will appear to remind you.
27.1.3.2.4. Kinematic Diffusivity Check Box: Kinematic Diffusivity
(applies only when Additional Variable Details: [Additional Variable name] check box: Option is
set to Transport Equation, Poisson Equation, Diffusive Transport Equation)
Enter a numerical quantity or CEL expression that specifies the value of the kinematic diffusivity
throughout the domain.
27.1.3.2.5. AV Properties for Fluid: Frame Overview
(applies only for homogeneous Additional Variables)
The settings contained in this frame are used to optionally specify the kinematic diffusivity of the selected
Additional Variable. The kinematic diffusivity may differ for each fluid in the domain. The solver calculates
a single effective kinematic diffusivity based on the kinematic diffusivity of the Additional Variable in
each fluid. For details, see Homogeneous Additional Variables in Multiphase Flow in the CFX-Solver
Theory Guide.
27.1.3.2.6. AV Properties for Fluid: List Box
This list box is used to select a fluid in the domain in order to optionally specify the kinematic diffusivity
of the selected Additional Variable in that fluid.
27.1.3.2.7. AV Properties for Fluid: [Fluid Name] Check Box
This check box determines whether or not the kinematic diffusivity of the selected Additional Variable
in the selected fluid is specified. Not specifying the kinematic diffusivity implies that the Additional
Variable is non-diffusive.
27.1.3.2.8. AV Properties for Fluid: [Fluid Name] Check Box: Kinematic Diffusivity
(applies only when Additional Variable Details: [Additional Variable name] Check Box: Option is
set to Homogeneous Transport Equation, Homogeneous Diffusive Transport Equation, or Homogeneous Poisson Equation)
Enter a numerical quantity or CEL expression that specifies the value of the kinematic diffusivity,
throughout the domain, of the selected Additional Variable in the selected fluid.
278
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Interface
27.1.3.2.9. Vector xValue, Vector yValue, and Vector zValue
(applies only when Additional Variable Details: [Additional Variable Name] Check Box: Option is
set to Vector Algebraic Equation)
Enter a numerical quantity or CEL expression for each vector algebraic equation component.
27.1.4. Boundary Details and Fluid Values Tabs for Boundary Condition Objects
The Boundary Details and Fluid Values tabs for a boundary condition object contain settings that
specify the values, fluxes, and transfer coefficients of Additional Variables at the boundary condition
location. These tabs are accessible, when applicable, by editing a boundary condition object.
The Additional Variables that require specification are those that have been applied to the domain (to
which the boundary condition belongs) in a form other than an algebraic equation.
For single phase flow, the Additional Variable settings are on the Boundary Details tab. For multiphase
flow, the Additional Variable settings for homogeneous Additional Variables are on the Boundary Details
tab and those for fluid-specific Additional Variables are either on the Boundary Details tab or the Fluid
Values tab.
The types of boundary conditions that may allow the specification of Additional Variables are:
•
Inlet
•
Opening
•
Wall
•
Outlet
27.1.4.1. Additional Variables: List Box
This list box is used to select an Additional Variable in order to set the details of its boundary condition
specification.
27.1.4.2. Additional Variables: [Name]
27.1.4.2.1. Option
•
Zero Flux
•
Value
•
Flux in
This option is applicable for Wall boundary conditions and, for Poisson and Diffusive transport
models, Inlet boundary conditions.
•
Transfer Coefficient
•
Wall Flux In
This option is applicable for multiphase flow only.
•
Wall Transfer Coefficient
This option is applicable for multiphase flow only.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
279
Chapter 27: Additional Variables
27.1.4.2.2. Value
(applies when Additional Variables: [Additional Variable Name]: Option is set to Value or Transfer
Coefficient)
27.1.4.2.3. Flux
(applies when Additional Variables: [Additional Variable Name]: Option is set to Flux in)
27.1.4.2.4. Transfer Coefficient
(applies when Additional Variables: [Additional Variable Name]: Option is set to Transfer Coefficient)
27.2. Creating an Additional Variable
1.
Click the Additional Variable icon
ditional Variable.
or select Insert > Expressions, Functions and Variables > Ad-
The Insert Additional Variable dialog box appears.
2.
Set Name to a unique name for the new Additional Variable. For details, see Valid Syntax for Named
Objects (p. 55).
3.
Click OK.
The Additional Variable details view opens on the Basic Settings tab.
4.
Specify the basic settings. For details, see Basic Settings Tab for Additional Variable Objects (p. 275).
5.
Click OK.
An object named after the Additional Variable is created and listed in the tree view under Expressions, Functions and Variables > Additional Variables.
280
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 28: Expressions
The Expressions workspace is used to generate and edit expressions using the CFX Expression Language
(CEL), which you can then use in CFX-Pre in place of almost any numeric value (as long as the correct
units are returned by the expression).
Note
In an expression, a term that has no units can be added to a term that has angular units, in
which case the software internally applies radians to the term that has no units.
Important
There is some CEL that works in CFX-Pre and CFX-Solver, but not in CFD-Post. Any expression
created in CFX-Pre and used as a Design Exploration output parameter could potentially
cause fatal errors during the Design Exploration run, so you should create all expressions for
Design Exploration output parameters in CFD-Post.
This chapter describes:
28.1. Expressions Workspace
28.2. Creating an Expression
28.3. Modifying an Expression
28.4. Importing or Exporting an Expression
28.1. Expressions Workspace
By double-clicking Expressions in the Outline workspace, or by inserting or editing an existing expression, the Expressions workspace opens in a new tab (see Figure 28.1 (p. 282)). This workspace consists
of a tree view and a details view. The following tabs are available in the details view:
•
Definition, used to edit the definition of an expression selected in the Expressions tree view. For details,
see Definition (p. 282).
•
Plot, used to plot an expression versus a variable. For details, see Plot (p. 283).
•
Evaluate, used to evaluate an expression when all quantities on which it depends are given. This is
useful for verifying that an expression is correctly specified. For details, see Evaluate (p. 283).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
281
Chapter 28: Expressions
Figure 28.1 Sample Expressions Workspace
28.1.1. Definition
CEL expressions can be defined using any combination of constants, variables, mathematical functions
and other CEL expressions. For details, see CFX Expression Language (CEL) in the CFX Reference Guide.
Tip
Right-clicking in the Definition window provides access to a list of all available variables,
expressions, locators, functions and constants. Although valid values can be chosen from
each of the various lists, the validity of the expression itself is not checked until you click
Apply.
Additional Variables can be used in expressions as soon as they have been completely specified. After they have been created, they appear in the list of available variables when rightclicking in the Definition window. For details, see:
•
CFX Expression Language (CEL) in the CFX Reference Guide
•
CEL Operators, Constants, and Expressions in the CFX Reference Guide.
Click Reset to undo changes made after opening the CEL expression for editing.
282
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating an Expression
28.1.2. Plot
The Plot tab is used to plot the selected expression against one variable. CFX-Pre automatically finds
the variables associated with an expression, even if the expression depends on another expression.
For example, when previewing the expression halfRadius, defined as 0.5*radius, where radius
is an expression that depends on the variables x and y, CFX-Pre presents x and y as the variables upon
which halfRadius depends.
1.
Set up an expression in the Definition tab, or open an existing expression. Click the Plot tab.
2.
Under Number of Points, set the number of sample data points for the plot.
Sample points are connected by line segments to approximate the functional relationship.
3.
Under Expression Variables, select the independent variable.
4.
Set the range for the independent variable.
5.
Set Fixed Value for all of the remaining independent variables.
6.
Click Plot Expression to view the resulting chart.
The Plot Expression button changes to Define Plot. This can be clicked after viewing the plot
in order to make adjustments to the plot specification.
28.1.3. Evaluate
The Evaluate tab is used to evaluate an expression when all variables upon which the equation depends
are specified. CFX-Pre automatically finds the variables associated with an expression, even if the expression depends on another expression.
For example, when previewing the expression halfRadius, defined as 0.5*radius, where radius
is an expression that depends on the variables x and y, CFX-Pre presents x and y as the variables upon
which halfRadius depends.
1.
Under Expression Variables, enter values for all listed variables.
2.
Click Evaluate Expression.
The resulting expression is evaluated using the given variable values.
28.2. Creating an Expression
1.
You can create an expression using any of the following methods:
•
On the Outline tab, right-click Expressions and select Insert > Expression.
•
Click Expression
•
Select Insert > Expressions, Functions and Variables > Expression from the menu bar.
in the main toolbar.
Whichever method you choose, the Insert Expression dialog box appears.
2.
Under Name, type a name for the new expression.
3.
Click OK.
4.
In the Expressions details view, under Definition, enter an expression. For details on using the
Definition area, see Definition (p. 282).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
283
Chapter 28: Expressions
5.
Click Apply.
6.
Optionally, select Plot or Evaluate to examine the expression.
28.3. Modifying an Expression
1.
In the Expressions tree view, double-click any expression, or right-click an expression and select Edit.
The Expression details view displays the definition of the expression.
2.
Under Definition, modify the expression. For details on using the Definition area, see Definition (p. 282).
3.
Make any desired changes and click Apply.
4.
Optionally, select Plot or Evaluate to examine the expression.
28.4. Importing or Exporting an Expression
Expressions can be imported and exported in simulations. For details, see:
•
Import CCL Command (p. 35)
•
Export CCL Command (p. 36).
Any number of CCL objects can be exported; this section describes exporting only expressions to a file.
28.4.1. Importing CCL Expressions
You can import expressions using the Import CCL function. For details, see Import CCL Command (p. 35).
1.
Select File > Import > CCL.
2.
Under Import Method, select Append or Replace.
Append imports expressions and overwrites any that currently exist in memory. Expressions that
do not match ones being imported are not changed. Replace deletes all expressions in memory
before importing.
3.
Select a location from which to import.
4.
Select a file to import.
5.
Click Open.
Important
Take care when importing CCL files because data can be overwritten.
28.4.2. Exporting CCL Expressions
You can export expressions using the Export CCL function. For details, see Export CCL Command (p. 36).
1.
Select File > Export > CCL from the main menu bar.
2.
Clear Save All Objects.
3.
Under Save All Objects, select LIBRARY > CEL > EXPRESSIONS.
4.
Select a location to which to export.
5.
Enter a name for the exported file.
284
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Importing or Exporting an Expression
6.
Click Save.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
285
286
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 29: User Functions
The User Function details view is used to create new interpolation functions (1D or 3D Cloud of Points),
and User CEL Functions. It is accessed from the Insert > Expressions, Functions and Variables > User
icon on the main toolbar.
Function or the User Function
User Function objects you create are listed under Expressions, Functions and Variables > User
Functions in the tree view.
The import of data from a file is discussed in the documentation for profile boundary conditions. For
details, see Profile Boundary Conditions in the CFX-Solver Modeling Guide.
After creating, modifying, or deleting functions, the CCL tree is checked for errors.
This chapter describes:
29.1. Interpolation Function
29.2. User Defined Function
29.1. Interpolation Function
This section describes:
•
One Dimensional Interpolation (p. 287)
•
Three Dimensional Interpolation (p. 288)
•
Importing Data from a File (p. 289)
29.1.1. One Dimensional Interpolation
1D interpolation functions can be used to specify any quantity in CFX-Pre for which a standard CEL
function (such as sin, cos, step, and so on) can be used. The function is created by interpolating
from a list of points and a list of values at those points.
For a 1D interpolation, you should set a single coordinate value and a single value associated with the
coordinate. You can also import data from a file. The coordinate and the value are interpreted in the
local coordinate frame, which will depend on where the function is used. For example, if the function
is used to set a boundary condition value, the coordinate frame selected for that boundary condition
will apply. For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
1.
Set Option to Interpolation (Data Input).
Additional information on the other function type is available in:
2.
•
Three Dimensional Interpolation (p. 288)
•
User Defined Function (p. 290).
Enter a single Argument Units.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
287
Chapter 29: User Functions
This will usually be a coordinate axis dimension (for example, m, cm, rad, and so on), but can be
any dimension. A variable using these units is passed to the interpolation function (for example,
x, y, r, z, and so on) when setting a quantity in CFX-Pre.
3.
Enter a single Result Units.
This unit should be a valid unit for the quantity you will be specifying (for example, type m s^1 for a velocity).
4.
Set Interpolation Data > Option to One Dimensional.
5.
Right-click in the window to import data from a file or delete an entry.
6.
Enter a single Coordinate value.
7.
Enter a Value associated with the Coordinate.
8.
Click Add to add the point value to the list (or Remove to remove a highlighted value from the list).
For details on the Extend Min and Extend Max options, see Extended Minimum and Maximum (p. 288).
The coordinate axis to which the coordinate value relates is determined by the argument passed when
calling the interpolation function. For example, for a Cartesian Velocity Component specified inlet, the
U component could be set to the expression MyInterpFunction(r), where MyInterpFunction
is the function name of the 1D Interpolation function, and r is the CFX radius system variable. The coordinate values you specify in this details view will then refer to values of r on the inlet boundary, and
the value would be the velocity value at each r location.
29.1.1.1. Extended Minimum and Maximum
The Extend Min and Extend Max options enable you to increase the valid range of the interpolation
function beyond the maximum or minimum specified coordinate values. The value the function will
take at coordinate values lower than the minimum specified coordinate, which is equal to the value at
the minimum specified coordinate. Similarly, the value at the maximum specified coordinate is extended
for higher coordinate values.
29.1.2. Three Dimensional Interpolation
Three dimensional functions can be used to specify any quantity in CFX-Pre for which a standard CEL
function (for example, sin, cos, step, and so on) can be used. The function is created by interpolating
values between a “cloud of points” using a distance weighted average based on the closest three points.
Common applications include setting an initial guess or a profile boundary condition from experimental
data values.
288
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Interpolation Function
For a three dimensional function, you should set X, Y, and Z coordinate values and a single value associated with the coordinate. The coordinates and the value are interpreted in the local coordinate frame,
which will depend on where the function is used. For example, if the function is used to set a boundary
condition value, the coordinate frame selected for that boundary condition will apply. For details, see
Coordinate Frames (p. 255) and Coordinate Frames in the CFX-Solver Modeling Guide. If the local coordinate
frame is cylindrical, the units for the Argument List should still be those of a Cartesian frame.
1.
Enter a unique function name that you will use when setting the value of a quantity using an expression.
2.
Argument Units: Enter a comma separated list of the units used for the coordinates.
These will usually be coordinate axis dimensions (for example, [m], [cm], and so on).
3.
Enter a single Result Units.
This unit should be a valid unit for the quantity you will be specifying (for example, [m s^-1]
for a velocity).
4.
Right-click in the window to import data from a file or delete an entry.
5.
Enter a comma, separating X, Y, Z coordinate values.
The coordinates are interpreted in the local coordinate frame, which will depend on where the
function is used.
6.
Enter a Value associated with the Coordinate.
7.
Click Add to add the point to the list (or Remove to remove a highlighted value from the list).
29.1.3. Importing Data from a File
After you create a user function (Insert > Expressions, Functions and Variables > User Function),
you see the function in the details view with the Option set to Interpolation (Data Input).
To import data from a file, set the Interpolation Data: Option as desired, then right-click in the Interpolation Data pane and select Import Data. This displays the Import Cloud Interpolation Data dialog
box.
•
For 1D data, Column Selection fields appear. You can select which column of data in your import file
is appropriate for the coordinates and values.
•
For 3D interpolations, columns are selected in the same way, with X, Y, and Z data all required.
29.1.4. Viewing and Editing Data Imported from a File
When you create a user function, it appears in the Outline view under Simulation > Expressions,
Functions and Variables > User Functions. Right-click the user function and select Edit to view and
edit the Basic Settings.
In the Basic Settings tab, the Value Field interacts with the Parameter List to control the variables
associated with each field.
To change the variables associated with a field:
1.
Select an element in the Value Field.
2.
Click the drop-down arrow beside the Parameter List field and select (or Ctrl-select) the variables that
you want to associate with the field you specified in the previous step. If the variable you want to select
to see all of the variables that are available.
does not appear, click Multi-select from extended list
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
289
Chapter 29: User Functions
29.2. User Defined Function
User CEL Functions are used in conjunction with User CEL Routines. A User Function must be created
after a User CEL Routine. For details, see User CEL Routines (p. 293). User Functions set the name of the
User CEL Routine associated with the function, the input arguments to pass to the routine and the expected return arguments from the routine.
1.
Select the User CEL Routine name (user routine name) from the drop-down list that the function will
apply to. For details, see Function Name (p. 290).
2.
Enter the input Argument Units list to pass to the subroutine.
For details, see Argument Units (p. 290).
3.
Enter the Result Units list output from the subroutine.
For details, see Result Units (p. 291).
29.2.1. Function Name
The function name is assigned when you create a new User CEL Function, and is equivalent to the name
you would set for an expression. You use this name, together with the input arguments, when setting
the expression for the quantity of interest. For details, see Defining Quantities with User CEL Functions (p. 290). The function name should follow usual naming rules (it may contain spaces but should
not include underscores).
29.2.1.1. Defining Quantities with User CEL Functions
After you have created a User CEL Function, you can use it to specify any quantity in CFX-Pre for which
a standard CEL function (for example, sin, cos, step, and so on) can be used. You should enter an expression using the notation:
<Function Name>(arg1[units], arg2[units], ...)
When using a system variable, an expression or a value, you do not need to specify units. For example,
a pipe inlet velocity profile might be set by entering:
inletvelocity(MaxVel, r, 0.2[m])
where inletvelocity is the function name of the User CEL Function, MaxVel is an existing expression
or value, r is a system variable and 0.2[m] corresponds to the pipe diameter.
You would enter the above expression as one of the velocity components at the inlet boundary condition
(you may also want to use it as a velocity component of the initial guess).
29.2.2. Argument Units
You should enter the units of each argument that you will be passing to the Subroutine. Units should
be comma separated and correspond to the order used when setting the expression for a quantity in
CFX-Pre. For example, enter [m], [m s^-1], [Pa] if you are passing a length, velocity and pressure value
to the subroutine. The values of arguments passed to a Subroutine are specified when you set an expression for a quantity in CFX-Pre. For details, see Defining Quantities with User CEL Functions (p. 290).
290
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Defined Function
29.2.3. Result Units
The result argument units are the units of the return arguments from the Subroutine. Units should be
comma separated and correspond to a valid unit for the quantity that you are specifying.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
291
292
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 30: User Routines
User routines are Fortran subroutines (User CEL Functions, Junction Box Routines, and Particle User
Routines) that you write for the CFX-Solver. You use the User Routine details view to create objects
that link your Fortran subroutines to the CFX-Solver. To access the User Routine details view, either
select Insert > Expressions, Functions and Variables > User Routines or click Insert User Routine
in the main toolbar.
Once your User Routines have been created and linked, they appear in the tree view under Simulation
> Expressions, Functions and Variables > User Routines.
Important
User routines cannot be used in the large memory partitioner.
User Routine Details View
The User Routine details view creates objects that link your Fortran subroutines to the CFX-Solver.
There are four types of user routines:
•
User CEL Routines (p. 293)
•
Junction Box Routines (p. 295)
•
Particle User Routines (p. 295)
•
For details on the fourth user-routine option, Transient Particle Diagnostics Routine,
refer to User Diagnostics Routine in the CFX-Solver Modeling Guide.
30.1. User CEL Routines
Available when Option is set to User CEL Function, User CEL Routines are used in conjunction
with User CEL Functions to define quantities in CFX-Pre based on a Fortran subroutine. The User CEL
Routine is used to set the calling name, the location of the subroutine, and the location of the Shared
Libraries associated with the subroutine.
1.
Enter the Calling Name (p. 294) of the subroutine within the subroutine file.
You should always use lowercase letters for this even when the subroutine name in the Fortran
file is in uppercase.
2.
Enter the Library Name and Library Path.
The library name will usually be your subroutine file name (without any extensions). The library
path is the path to the directory containing the system dependent directories and supports lists
of paths. For details, see Library Name and Library Path (p. 294).
User CEL Functions are created after the associated routine has been defined. For details, see:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
293
Chapter 30: User Routines
•
User Defined Function (p. 290)
•
User CEL Functions and Routines in the CFX-Solver Modeling Guide.
30.1.1. Calling Name
The Calling Name is the name of the subroutine within a Fortran file. This name appears immediately
after the SUBROUTINE statement in a Fortran file. It is usually in upper case in the Fortran file, but
should always be entered in lower case. It must not include spaces but may contain underscores (this
is different from the usual naming rules).
30.1.2. Library Name and Library Path
This is the name of the shared library. The Library Name will be the name of the file containing the
subroutine, ignoring any file extensions (for example, InletProfile for the file named InletProfile.F). The file name depends on how you ran the cfx5mkext command:
•
If you did not specify a -name option when running the cfx5mkext command, the file name will be
the name of your shared library. For details, see Shared Libraries in the CFX-Solver Modeling Guide.
•
If you did specify the -name option when running the cfx5mkext command, the file name will be
the name you specified.
Note that if you look at the actual file name of the shared library, it will have a lib prefix (UNIX only)
and either a .so, .sl, or .dll suffix depending on your platform. Do not include the prefix or suffix
in the Library Name.
The Library Path is the absolute path to the directory that contains the shared libraries in subdirectories
for each platform. The path name depends on how you ran the cfx5mkext command:
•
If you did not specify a -dest option when running the cfx5mkext command, this will be the path
to the directory in which the cfx5mkext command was executed. For details, see Shared Libraries in
the CFX-Solver Modeling Guide.
•
If you did specify the “-dest” option when running the cfx5mkext command, the path name will
be the name you specified.
On UNIX platforms, the Library Path will look like:
/home/user/SharedLibraries
On Windows systems, the Library Path will look like:
F:\user\SharedLibraries
If you are running in parallel and specify only a single library path, then each machine should be able
to locate the shared libraries using the specified Library Path. On Windows systems, you may have to
map network drives so that the path to the libraries is the same on each machine. However, you can
also specify the Library Path as a list. ANSYS CFX will try to locate your shared libraries on each machine
in the parallel run using the list of paths provided. Comma (,), colon (:) and semi-colon (;) separated
lists are valid. For example, when running in parallel across Windows and UNIX machines, a valid path
may look like:
/home/user/SharedLibraries, C:\Shared Libraries
The colon used after a Windows drive letter is treated correctly and is not interpreted as a list separator.
294
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Particle User Routines
30.2. Junction Box Routines
Junction box routines are used to call your own Fortran subroutines during execution of the CFX-Solver.
You must create a junction box routine object so that the CFX-Solver knows the location of the subroutine, the location of the shared libraries associated with the subroutine, and when to call the subroutine. Each of these items is specified in the details view. For details, see User Junction Box Routines
in the CFX-Solver Modeling Guide.
To complete the Junction Box Routine details:
1.
The first three parameters are identical to those described for the User Function option, under
Calling Name (p. 294) and Library Name and Library Path (p. 294).
2.
Enter the Junction Box Location at which to call the subroutine. For details, see Junction Box Routine
Options and Parameters in the CFX-Solver Modeling Guide.
Junction box routines appear in the LIBRARY section of a CCL file. You can create many junction box
routines in CFX-Pre, but only call the required routines during execution of the CFX-Solver. This enables
you to read in a CCL file containing a list of junction box routines and then select only those that you
want to call. This selection is made on the Solver Control tab. For details, see Basic Settings Tab (p. 199).
30.3. Particle User Routines
Particle user routines are used to create user defined injection regions and particle user sources. Creating
a user routine with the Particle User Routine option selected is identical to creating a routine
with the User CEL Function option selected. For details, see:
•
User CEL Routines (p. 293)
•
Particle Injection Regions Tab (p. 131)
•
Particle User Sources in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
295
296
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 31: Simulation Control
Simulation controls allow you to define the execution of analyses and related tasks like remeshing in
the simulation. Specific controls include definitions of global execution and termination controls and
one or more configurations. Additional information regarding these topics are provided in Execution
Control (p. 299) and Configurations (p. 307), respectively.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
297
298
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 32: Execution and Termination Control
This chapter describes:
32.1. Execution Control
32.2.Termination Control
32.1. Execution Control
The Execution Control settings described below apply to all configurations in the simulation. You can
override these settings for any configuration from the Run Definition tab on the details view of the
Configuration (for details, see Run Definition Tab (p. 313)) or the Define Run dialog box in the CFXSolver Manager (for details, see The Define Run Dialog Box in the CFX-Solver Manager User's Guide).
This section describes:
32.1.1. Overview of Defining CFX-Solver Startup
32.1.2.The Details View for Execution Control
32.1.1. Overview of Defining CFX-Solver Startup
To define how a CFX-Solver can be started, the number of settings that you need to set up for Execution
Control depends on the case:
•
In some cases, you need to specify only the name of a CFX-Solver input file (*.def or *.mdef). For
cases that require initialization from previous results, you also need to specify the name of a results file
(*.res).
•
You can configure runs in serial or parallel:
•
–
Serial run is the default way of running a CFD case. During a serial run, all computation is done by
a single process running on one processor.
–
Parallel run partitions the computation into more than one process and is done on more than one
processor in a single machine (local parallel processing) or on more than one machine (distributed
parallel processing). You also have the option of specifying how the computation is partitioned for
a parallel run.
You can optionally select the system priority for the interpolator and solver computation as well as
settings such as precision and memory allocation.
When you have finished defining how CFX-Solver will start, click OK or Apply to save the settings.
Details of the above steps are described in the next section.
32.1.2. The Details View for Execution Control
You access the details view for Execution Control from CFX-Pre by clicking Insert > Solver > Execution
Control or by right-clicking on Simulation Control in the details view and selecting Insert > Execution
Control.
The tabs presented in the details view for Execution Control are described in the following sections:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
299
Chapter 32: Execution and Termination Control
•
Run Definition Tab (p. 300)
•
Partitioner Tab (p. 301)
•
Solver Tab (p. 304)
•
Interpolator Tab (p. 304)
32.1.2.1. Solver Input File Name
Ensure that the name of a CFX-Solver input file (extension .def or .mdef) is specified under Solver
Input File.
32.1.2.2. Run Definition Tab
1.
Select Initial Values Specification so that you can specify one or more sources of initial values. Note
that for cases with multiple configurations, initial values specifications are not valid for Global Settings.
For each source of initial values (most runs only require one), do the following:
a.
Click New
b.
Select an initial values object from the list and select either the Results File or Configuration
Results option for Initial Values > Option.
to create an initial values object.
1.
If you selected the Results File option, then specify the file name of a file from which initial
values should be used.
2.
If you selected the Configuration Results option, then specify the name of the configuration
from which initial values should be used. Note that this option is only available in the context
of multi-configuration simulations. It allows the introduction of dependencies on initial values
that will become available at run time.
c.
The Use Mesh From setting determines which mesh is used for the analysis: the one specified in
the Solver Input File option, or the one in the Initial Values. The mesh from the Initial Values
File can only be used in a limited set of circumstances. See Using the Mesh from the Initial Values
File in the CFX-Solver Modeling Guide for details.
d.
Select Continue History From if you want to continue the run history (convergence history,
monitor plots, time and time step counters, etc…) and use the smoothest restart possible from
the selected Initial Values File. The run will continue from the one contained the specified initial
values object. Note that the run history will reset if Continue History From is not selected.
Full details of the settings can be found in Reading the Initial Conditions from a File in the CFXSolver Modeling Guide.
2.
3.
300
Set Type of Run to Full or Partitioner Only.
•
Full runs the partitioner if applicable, and then runs Solver.
•
Partitioner Only is used for parallel runs only and does not run Solver. This writes a .par
file.
Select or clear Double Precision. This setting will determine the default (single or double) precision
of the partitioner, solver and interpolator executables. For details on the precision of executables, see
Double-Precision Executables in the CFX-Solver Manager User's Guide. The precisions of the partitioner,
solver, and interpolator executables can be set individually on the Partitioner, Solver, and Interpolator tabs.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Execution Control
4.
Configure the Parallel Environment as required.
5.
If required, under Run Environment, set the working directory.
6.
If required, select Show Advanced Controls to display other tabs.
Additional information is provided in the next section, Parallel Environment, and in Initial Condition
Modeling in the CFX-Solver Modeling Guide.
Parallel Environment
For a distributed parallel setup, specify the number of partitions assigned to each host. If choosing a
specified partition weighting (under Partitioner), click directly on the partition weight number to edit
it. There should be one weight entry per partition.
1.
Under Parallel Environment, select a Run Mode.
2.
Configure the mode as required.
Run Mode determines whether the run is serial (the default when defining a run in which a
problem solved as one process), or parallel (problem split into partitions).
•
A serial run (the default) requires no additional configuration
•
To learn how to configure a parallel run, see Parallel Run in the CFX-Solver Manager User's Guide.
32.1.2.2.1. Mesh Node Reordering
You can change the order of the nodes in the mesh. Depending on the case this reordering may result
in a reduction in the run time for the CFX-Solver. From Mesh Options > Node Reordering > Options,
you can select None, Cuthill McKee and Reverse Cuthill McKee.
32.1.2.2.2. Optional Quitting CFX-Pre
Optionally, you can elect to have CFX-Pre quit upon writing CFX-Solver Input file.
32.1.2.3. Partitioner Tab
Use the Partitioner tab to configure the mesh partitioning options.
Note
An existing partition file cannot be used if the simulation involves either the Monte Carlo or
Discrete Transfer radiation models.
Partitions may be viewed prior to running CFX-Solver. For details, see CFX Partition File in the CFXSolver Manager User's Guide.
1.
Select the Partitioner tab.
If this is not available, ensure Show Advanced Controls is selected in the Run Definition tab.
2.
If required, under Initial Partition File, click Browse
and select the partition file to load.
The *.par file is only required if a model has already been partitioned. The number of partitions
in the partitioning file must be the same as that selected on the Run Definition tab.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
301
Chapter 32: Execution and Termination Control
Note
A partition file generated in ANSYS CFX 11.0 or earlier versions is not supported in
ANSYS CFX 12.0. If such a file is used in ANSYS CFX 12.0, then an error message is
generated.
3.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities, see
The cfx5control Application in the CFX-Solver Manager User's Guide.
4.
Optionally, set the precision: under Executable Settings, select Override Default Precision and choose
either Single or Double. This setting for the partitioner will override the corresponding specification,
if set, on the Run Definition tab.
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
5.
If required, select the Use Large Problem Partitioner option, which is available on 64-bit platforms
only. This option starts the large problem partitioner which can partition problems up to 2^31-1 elements. This partitioner uses 64-bit integer and logical variables so it will allocate more memory than
the default partitioning executable. For details, see Large Problem Partitioner Executables in the CFXSolver Manager User's Guide.
6.
Under Partitioning Detail, choose a Partition Type and configure it.
Depending on the selected partition type, various options must be configured. Partition types
include:
•
Multilevel Graph Partitioning Software - MeTiS in the CFX-Solver Modeling Guide. When first running
in parallel, it is recommended that Partition Type be set to MeTiS.
•
Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
Optimized Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
Directional Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
User Specified Direction in the CFX-Solver Modeling Guide
•
Simple Assignment in the CFX-Solver Modeling Guide
•
Radial in the CFX-Solver Modeling Guide
•
Circumferential in the CFX-Solver Modeling Guide
7.
If required, configure the Partition Weighting as described below.
8.
If required, configure the Multidomain Option. You can select from the following options:
•
Independent Partitioning: Each domain is partitioned independently into the specified
number of partitions.
•
Coupled Partitioning: All domains that are connected together are partitioned together.
Note that solid domains are still partitioned separately from fluid/porous domains. Coupled partitioning often leads to better scalability, reduced memory requirements, and sometimes better robustness, than independent partitioning because there are fewer partition boundaries.
For details, see Selection of the Partitioning Mode for Multi-Domain Cases in the CFX-Solver
Modeling Guide.
302
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Execution Control
When the coupled partitioning option is activated, you can further choose to set the Multipass
Partitioning option. The Transient Rotor Stator option is relevant only for simulations
having transient rotor stator interfaces. It uses a special multipass algorithm to further optimize
the partition boundaries. This approach generates circumferentially-banded partitions adjacent
to each transient rotor stator interface, which ensures that interface nodes remain in the same
partition as the two domains slide relative to each other. Away from the interface, the partitioning is handled using whichever method is specified for the Partition Type.
Performance of particle transport calculations may be made worse when using coupled partitioning.
9.
If required, under Partitioner Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
Partitioning Weighting
As discussed below, partitions can be weighted in different ways. The default setting is Automatic.
•
Uniform
•
Specified
•
Automatic
Uniform
Assigns equal-sized partitions to each process.
Specified
Requires Run Definition to be configured with individual partition weights.
Partition Weights is added to the parallel environment. This allows partition weights to be entered.
When more than one partition is assigned to any machine, the number of partition weight entries must
equal the number of partitions. The partition weight entries should be entered as a comma-separated
list. For a distributed run like the following:
Host
# of Partitions
Partition Weights
Sys01
1
2
Sys02
2
2, 1.5
Sys03
1
1
Sys01 is therefore a single partition and the weight is 2. Sys02 has two partitions and they are individually weighted at 2 and 1.5. The final system has a single partition with a weight of 1.
If partition weight factors are used, the ratio of partition weights assigned to each partition controls
the partition size.
Once started, the run progresses through the partitioning, and then into the solution of the CFD problem.
Extra information is stored in the CFX output file for a parallel run. For details, see Partitioning Information in the CFX-Solver Manager User's Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
303
Chapter 32: Execution and Termination Control
Automatic
Calculates partition sizes based on the Relative Speed entry specified for each machine in the
hostinfo.ccl file.
Machines with a faster relative speed than others are assigned proportionally larger partition sizes. The
entry of relative speed values is usually carried out during the CFX installation process, and accurate
entries for relative speed can significantly optimize parallel performance.
32.1.2.4. Solver Tab
1.
Select the Solver tab.
If this is not available, ensure Show Advanced Controls in the Run Definition tab is selected.
2.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities as well
as how you can change them after the execution of the solver has started, see The cfx5control Application in the CFX-Solver Manager User's Guide.
3.
If required, from Double Precision Override or Executable Settings > Double Precision Override,
select or clear Double Precision. This setting for the solver will override the corresponding specification,
if set, on the Run Definition tab.
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
4.
If required, under Solver Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
32.1.2.5. Interpolator Tab
1.
Select the Interpolator tab.
If this is not available, ensure Show Advanced Controls in the Run Definition tab is selected.
2.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities, see
The cfx5control Application in the CFX-Solver Manager User's Guide.
3.
Optionally, set the precision: under Executable Settings, select Override Default Precision and choose
either Single or Double. This setting for the interpolator will override the corresponding specification,
if set, on the Run Definition tab.
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
4.
If required, under Interpolator Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
32.2. Termination Control
The Termination Control settings apply to the simulations with one or more configurations. This section
describes:
32.2.1. Overview of Configuration Termination
32.2.2. Details View for Termination Control
32.2.1. Overview of Configuration Termination
Many simulations with one or more configurations will terminate naturally without explicitly introducing
Termination Control. However, in some cases explicit Termination Control is required. For example,
304
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Termination Control
consider a case where a simulation has a sequence of configurations that are set up to run one after
the other with the sequence to then return to the first configuration in the sequence (this could occur
when modeling an internal combustion engine where there could be a configuration for each of the
intake, compression, power and exhaust strokes and the simulation repeatedly cycles through each of
the four configurations). There can be one or more conditions for terminating a simulation. Each termination condition can be based on the number of times a configuration has been executed or whenever
a CFX-Solver interrupt condition for a configuration has been satisfied.
To define the conditions under which a simulation should be terminated you need to:
1.
If required, create one or more termination Control Conditions.
2.
For each Control Condition, select the appropriate termination control Option.
3.
For each Control Condition set the Configuration Name appropriate for the termination control
condition.
4.
For each Control Condition, set the appropriate Number of Steps or Condition Name(s).
When you have finished defining how the simulation will terminate, click OK or Apply to save the settings.
Details of the above steps are described in the next section.
32.2.2. Details View for Termination Control
You access the details view for Termination Control from CFX-Pre by clicking Insert > Configurations
> Termination Control or by right-clicking on Simulation Control in the details view and selecting
Insert > Termination Control.
The following describes the details of the Termination Control tab.
Control Conditions
A list displaying the available termination control conditions. Click Add new item
to add a new ter-
mination control condition. To change its settings, the termination control condition must be highlighted.
You can highlight a condition by selecting it from the displayed list. Click Delete
to delete a highlighted
termination control condition.
Control Condition: Options
The options for termination control are either Max. Configuration Steps or Solver Interrupt Conditions.
The former setting is used to terminate a simulations after a selected configuration has been executed
the prescribed number of times. The latter setting is used to terminate a simulation whenever the named
CFX-Solver interrupt conditions for the selected configurations have been satisfied. Note that the latter
option is only valid if CFX-Solver interrupt conditions have been defined. For details, see Interrupt Control (p. 200).
Control Condition: Configuration Name
Choose the configuration for which the termination control is to be applied.
Control Condition: Number of Steps
This setting is used to set to the maximum number of times the specified configuration is to be executed
in the course of the simulation.
Control Condition: Condition Name(s)
This setting is used to identify the names of the solver interrupt condition for the specified configuration
to be used to terminate the simulation.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
305
306
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 33: Configurations
This chapter describes how to control the sequencing of configurations for a simulation, how to define
when remeshing is required, and procedures for defining how CFX-Solver can be started for a configuration. The Configuration settings described below apply to a specified flow analyses in the simulation.
This chapter describes:
33.1. Overview of Defining a Configuration
33.2.The Details View for Configuration
33.1. Overview of Defining a Configuration
To set up the sequencing of configurations in a simulation, you need to define a configuration for each
step in the simulation. Typically, there is a configuration for each analysis in the simulation. You are
required to define at least one activation condition for each configuration. You set up the desired sequencing of configurations in a simulation by your choice of activation conditions. For each required
configuration:
1.
Create the configuration.
2.
Set the name of the analysis to be associated with the configuration.
3.
Create the required number of activation controls for the configuration.
4.
Set the activation control option to activate the configuration at the start of the simulation or
following the completion of another configuration.
Note that it is possible to have more than one configuration activated at the start of the simulation.
You also have the option of specifying more than one activation condition for a configuration (for example, a configuration can be activated at the start of the simulation as well as at the completion of
another configuration).
To control when remeshing is to occur, you are required to:
1.
Create a remeshing definition.
2.
Select the appropriate remeshing option.
3.
Set up the remeshing activation condition.
4.
Identify the location where the remeshing is to occur.
5.
Supply any additional information required by the selected remeshing option.
To define how a CFX-Solver can be started, the number of settings that you need to define for Configuration depends on the case:
•
In some cases, you need only to specify the name of a CFX-Solver input file (*.def or *.mdef). For
cases that require initialization from previous results, you also need to specify the name of a results file
(*.res).
•
You can configure runs in serial or parallel:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
307
Chapter 33: Configurations
•
–
Serial run is the default way of running a CFD case. During a serial run, all computation is done by
a single process running on one processor.
–
Parallel run partitions the computation into more than one process and is done on more than one
processor in a single machine (local parallel processing) or on more than one machine (distributed
parallel processing). You also have the option of specifying how the computation is partitioned for
a parallel run.
You can optionally select the system priority for the interpolator and solver computation as well as
settings such as precision and memory allocation.
When you have finished setting the parameters for the configuration, click OK or Apply to save the
settings.
Details of the above steps are described in the next section.
33.2. The Details View for Configuration
You access the details view for a configuration in CFX-Pre by double-clicking its Simulation Control >
Configurations entry in the Outline view or by right-clicking its Simulation Control > Configurations
entry in the Outline view and selecting Edit.
The tabs presented in the details view for the configurations are described in the following sections:
•
General Settings Tab (p. 308)
•
Remeshing Tab (p. 309)
•
Run Definition Tab (p. 313)
•
Partitioner Tab (p. 314)
•
Solver Tab (p. 316)
•
Interpolator Tab (p. 317)
33.2.1. General Settings Tab
The General Settings tab for a configurations requires that you:
1.
Select the Flow Analysis for the configuration.
2.
Define at least one Activation Condition. There are two Option values available for each Activation
Condition:
•
Start of Simulation to activate the configuration at the start of the simulation.
•
End of Configuration to activate the configuration whenever any one of a prescribed configuration
completes.
One activation condition is automatically generated for you and the default Option is set to Start of
Simulation. If required, create additional activation conditions by clicking New
. To change the
settings for an activation condition or to delete a condition (by clicking Delete
), you must highlight
a condition by selecting it from the displayed list.
308
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Configuration
33.2.2. Remeshing Tab
The Remeshing tab allows to you introduce one or more remeshing definitions within the configuration
being edited. To create a remeshing definition, click New
Guide in the CFX Reference Guide.
. For additional details, see Remeshing
Each remeshing definition requires that you:
1.
Select either the User Defined or ICEM CFD Replay value for the Option setting. Additional settings, which depend on the option selected, are described in the sections User Defined Remeshing (p. 310) and ANSYS ICEM CFD Replay Remeshing (p. 311), presented below.
2.
Select one or more activation condition(s) to be used to activate the remeshing object during the
configuration’s execution. This selection is made from a list of the solver Interrupt Control conditions (for details, see Interrupt Control (p. 200)) that were defined for the Flow Analysis specified
in the General Settings tab.
3.
Select the mesh Location that will be replaced by remeshing. This selection is made from a list
of the 3D mesh regions that are used in the Flow Analysis specified in the General Settings tab.
Each remeshing definition also allows you to specify a comma separated list of Mesh Reload Options
that control how the new mesh replaces the previous one. The new mesh could, for example, be reloaded
as a .gtm file using [mm] length units and all relevant mesh transformations by specifying:
Mesh Reload Options = "replacetype=GTM,replaceunits=mm,notransform=false"
These and other options are summarized in the table below.
Table 33.1 Reload Options
Reload
Option
Description and Values
notransform
True (default) ensures mesh transformations are not performed on mesh reload.
replacetype
True or False
Type of replacement mesh file.
ANSYS: cdb and inp files
CFX4: geo files
CFX5: CFX 5.1 files
CGNS: cgns and cgn files
GEM: TfC files
GTM: gtm files
GtmDirect: def and res files
GTM_DSDB: ANSYS cmdb and dsdb files
Def: def files that are older than CFX 5.6 (or if duplicate node removal is required)
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
309
Chapter 33: Configurations
Reload
Option
Description and Values
Fluent: cas and msh files
Generic: ICEM CFD mesh (cfx, cfx5, msh) files
GRD: CFX-TASCflow (grd) files
IDEAS: unv files
MSC: Patran out and neu files
PDC: GridPro files
replacegenargs
Generic mesh import options (as space separated list):
-g: Ignore degenerate element errors
-n: Do not do duplicate node removal
-T: specify duplicate node removal tolerance (float).
-D: Primitive naming strategy ; either Standard Naming Strategy or Derived
Naming Strategy.
replacespecargs
Space-separated list of type-specific import arguments, as discussed in Supported
Mesh File Types (p. 67)
replaceunits
Length units of the replacement mesh.
micron, mm, cm, m, in, ft
33.2.2.1. User Defined Remeshing
Full control over how the replacement mesh is generated is provided by the User Defined remeshing
option. When this option is used, a user-defined command is required to gather all input data needed
for remeshing and for create the replacement mesh file. The CFX-Solver, however, automatically executes
the following tasks:
•
Import the new mesh into the problem definition
•
Interpolate solution data from the previous mesh onto the new mesh
•
Repartition the new mesh if a parallel run mode is used
•
Restart the equation solution process.
In addition to the required and optional general settings described above, the User Defined option
requires specification of:
•
An External Command that is responsible for generating a replacement mesh file
•
The name of the Replacement File.
The External Command is submitted to the operating system for execution. This may be a command
to start a mesh (re)generation executable directly with certain inputs, or a shell script that executes
several commands. It is important to note that this command is submitted from the current run directory
(for example case_001.dir), so care is required when using relative paths to files during remeshing.
310
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Configuration
Useful inputs to the remeshing process may be extracted from the most recently generated CFX-Solver
Results file. For details, see Remeshing Guide in the CFX Reference Guide. This file is located in the run
directory, and is simply called res (no prefix or suffix) at the time of submitting the External Command
to the operating system.
For additional details, see User Defined Remeshing in the CFX Reference Guide.
33.2.2.2. ANSYS ICEM CFD Replay Remeshing
Remeshing using the ANSYS ICEM CFD mesh generator is highly automated when the ICEM CFD Replay
remeshing option is used. This is accomplished by combining settings made in the Flow Analysis
(specified on the configuration’s General Settings tab) with a batch run of the ANSYS ICEM CFD mesh
generator using replay (session) files.
When this option is used the CFX-Solver automatically executes the following tasks:
•
Compile a comprehensive remeshing replay file from a combination of provided and user-specified
replay files
•
Execute the ANSYS ICEM CFD mesh generator in batch mode, using the remeshing replay file
•
Import the new mesh into the problem definition
•
Interpolate solution data from the previous mesh onto the new mesh
•
Repartition the new mesh if a parallel run mode is used
•
Restart the equation solution process.
In addition to the required and optional general settings described above, the ICEM CFD Replay option
requires specification of:
•
An ANSYS ICEM CFD Geometry File (with a tin extension) that contains the reference geometry
•
A Mesh Replay File (with an rpl extension) that contains a recording of the steps (that is, the
commands) used to generate the mesh in the ANSYS ICEM CFD application.
Additional, optional settings include:
•
ICEM CFD Geometry Control definitions
•
ICEM CFD Mesh Control definitions
•
Scalar Parameter definitions.
For additional details, see ICEM CFD Replay Remeshing in the CFX Reference Guide.
33.2.2.2.1. ICEM CFD Geometry Control
Option settings for ICEM CFD Geometry Control other than None are used to modify the reference
geometry contained in the ICEM CFD Geometry File according to the mesh motion specifications defined
in the CFX case setup. If the geometry control option is set to Automatic, then one or more ICEM CFD
Part Map definitions may be defined. Each definition provides a mapping between:
•
An ICEM CFD Parts List, which is a list of parts (or families) defined in the referenced Geometry
File
•
The translation of the centroid of a Boundary defined in the Flow Analysis.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
311
Chapter 33: Configurations
These definitions are applied, in conjunction with the default geometry control replay file (icemcfd_GeomCtrl.rpl contained the <CFXROOT>/etc/Remeshing directory), to modify the reference geometry
prior to regenerating the mesh. If the geometry control option is set to User Defined Replay File, then
a File Name is required and the specified file is used instead of the default geometry control replay
file.
33.2.2.2.2. ICEM CFD Mesh Control
Options settings for ICEM CFD Mesh Control other than None are used to set values of some predefined parameters used by ANSYS ICEM CFD during remeshing. If the mesh control option is set to
Automatic, then one or more ICEM CFD Part Parameter definitions may be defined. Each definition
provides a mapping for an ICEM CFD Parameter that governs mesh attributes like the maximum element
size (emax) or the maximum element height (ehgt), between:
•
An ICEM CFD Parts List, which is a list of parts (or families) defined in the referenced Geometry
File
•
A Monitor Point defined in the Flow Analysis.
These definitions are applied in conjunction with the default mesh control replay file (icemcfd_MeshCtrl.rpl contained the <CFXROOT>/etc/Remeshing directory), to modify the reference geometry
prior to regenerating the mesh. If the mesh control option is set to User Defined Replay File, then a
File Name is required and the specified file is used instead of the default mesh control replay file.
33.2.2.2.3. Scalar Parameter
Scalar Parameter definitions are used to set values of additional pre- or user-defined parameters referenced in any of the replay files used by ANSYS ICEM CFD during remeshing. Each definition provides
a mapping between a scalar parameter used during remeshing (with the same name as the Scalar
Parameter definition) and a Monitor Point defined in the Flow Analysis.
The parameters listed in the table below are used in the default geometry control replay file, and become
relevant if a Scalar Parameter definition is created with the same name.
Table 33.2 Scalar Parameters
Scalar Parameter
Description
ICEM CFD Geometry Scale
The specified scale is used to address length unit differences
between the geometry contained in the specified ANSYS ICEM
CFD Geometry File and the mesh contained in the CFX-Solver
Input file. For example, if the length unit is [mm] in the ANSYS
ICEM CFD geometry and [m] in the CFX-Solver InputCFX-Solver
Input file, then the geometry scale should be set to 0.001.
OFFSET X PartName
The specified offset values are added to the centroid displacements (see the discussion on ICEM CFD Geometry Control
presented above) that are applied for the part (or family)
named PartName. Note that the ICEM CFD Geometry Scale
is also applied to the offset specified offset.
OFFSET Y PartName
OFFSET Z PartName
312
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Configuration
33.2.3. Run Definition Tab
The Run Definition tab settings described below apply to a specified configuration in the simulation.
You can override these settings for the specific configuration from the Define Run dialog box in the
CFX-Solver Manager (for details, see The Define Run Dialog Box in the CFX-Solver Manager User's Guide).
1.
Select Initial Values Specification so that you can specify one or more sources of initial values. Note
that for cases with multiple configurations, initial values specifications are not valid for Global Settings.
For each source of initial values (most runs only require one), do the following:
a.
Click New
b.
Select an initial values object from the list and select either the Results File or Configuration
Results option for Initial Values > Option.
to create an initial values object.
1.
If you selected the Results File option, then specify the file name of a file from which initial
values should be used.
2.
If you selected the Configuration Results option, then specify the name of the configuration
from which initial values should be used. Note that this option is only available in the context
of multi-configuration simulations. It allows the introduction of dependencies on initial values
that will become available at run time.
c.
The Use Mesh From setting determines which mesh is used for the analysis: the one specified in
the Solver Input File option, or the one in the Initial Values. The mesh from the Initial Values
File can only be used in a limited set of circumstances. See Using the Mesh from the Initial Values
File in the CFX-Solver Modeling Guide for details.
d.
Select Continue History From if you want to continue the run history (convergence history,
monitor plots, time and time step counters, etc…) and use the smoothest restart possible from
the selected Initial Values File. The run will continue from the one contained the specified initial
values object. Note that the run history will reset if Continue History From is not selected.
Full details of the settings can be found in Reading the Initial Conditions from a File in the CFXSolver Modeling Guide.
2.
Set Type of Run to Full or Partitioner Only.
•
Full runs the partitioner if applicable, and then runs Solver.
•
Partitioner Only is used for parallel runs only and does not run Solver. This writes a .par
file.
3.
Select or clear Double Precision. This setting will determine the default (single or double) precision
of the partitioner, solver and interpolator executables. For details on the precision of executables, see
Double-Precision Executables in the CFX-Solver Manager User's Guide. The precisions of the partitioner,
solver, and interpolator executables can be set individually on the Partitioner, Solver, and Interpolator tabs.
4.
Configure the Parallel Environment as required.
5.
If required, under Run Environment, set the working directory.
6.
If required, select Show Advanced Controls to display other tabs.
Additional information is provided in the next section, Parallel Environment, and in Initial Condition
Modeling in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
313
Chapter 33: Configurations
Parallel Environment
For a distributed parallel setup, specify the number of partitions assigned to each host. If choosing a
specified partition weighting (under Partitioner), click directly on the partition weight number to edit
it. There should be one weight entry per partition.
1.
Under Parallel Environment, select a Run Mode.
2.
Configure the mode as required.
Run Mode determines whether the run is serial (the default when defining a run in which a
problem solved as one process), or parallel (problem split into partitions).
•
A serial run (the default) requires no additional configuration
•
To learn how to configure a parallel run, see Parallel Run in the CFX-Solver Manager User's Guide.
33.2.4. Partitioner Tab
The Partitioner Tab settings described below apply to a specified configuration in the simulation. You
can override these settings for the specific configuration from the Define Run dialog box in the CFXSolver Manager (for details, see The Define Run Dialog Box in the CFX-Solver Manager User's Guide).
Use the Partitioner tab to configure the mesh partitioning options.
Note
An existing partition file cannot be used if the simulation involves either the Monte Carlo or
Discrete Transfer radiation models.
Partitions may be viewed prior to running CFX-Solver. For details, see CFX Partition File in the CFXSolver Manager User's Guide.
1.
Select the Partitioner tab.
If this is not available, ensure Show Advanced Controls is selected in the Run Definition tab.
2.
If required, under Initial Partition File, click Browse
and select the partition file to load.
The *.par file is only required if a model has already been partitioned. The number of partitions
in the partitioning file must be the same as that selected on the Run Definition tab.
Note
A partition file generated in ANSYS CFX 11.0 or earlier versions is not supported in
ANSYS CFX 12.0. If such a file is used in ANSYS CFX 12.0, then an error message is
generated.
3.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities, see
The cfx5control Application in the CFX-Solver Manager User's Guide.
4.
Optionally, set the precision: under Executable Settings, select Override Default Precision and choose
either Single or Double. This setting for the partitioner will override the corresponding specification,
if set, on the Run Definition tab.
314
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Configuration
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
5.
If required, select the Use Large Problem Partitioner option, which is available on 64-bit platforms
only. This option starts the large problem partitioner which can partition problems up to 2^31-1 elements. This partitioner uses 64-bit integer and logical variables so it will allocate more memory than
the default partitioning executable. For details, see Large Problem Partitioner Executables in the CFXSolver Manager User's Guide.
6.
Under Partitioning Detail, choose a Partition Type and configure it.
Depending on the selected partition type, various options must be configured. Partition types
include:
•
Multilevel Graph Partitioning Software - MeTiS in the CFX-Solver Modeling Guide. When first running
in parallel, it is recommended that Partition Type be set to MeTiS.
•
Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
Optimized Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
Directional Recursive Coordinate Bisection in the CFX-Solver Modeling Guide
•
User Specified Direction in the CFX-Solver Modeling Guide
•
Simple Assignment in the CFX-Solver Modeling Guide
•
Radial in the CFX-Solver Modeling Guide
•
Circumferential in the CFX-Solver Modeling Guide
7.
If required, configure the Partition Weighting as described below.
8.
If required, configure the Multidomain Option. You can select from the following options:
•
Independent Partitioning: Each domain is partitioned independently into the specified
number of partitions.
•
Coupled Partitioning: All domains that are connected together are partitioned together.
Note that solid domains are still partitioned separately from fluid/porous domains. Coupled partitioning often leads to better scalability, reduced memory requirements, and sometimes better robustness, than independent partitioning because there are fewer partition boundaries.
For details, see Selection of the Partitioning Mode for Multi-Domain Cases in the CFX-Solver
Modeling Guide.
When the coupled partitioning option is activated, you can further choose to set the Multipass
Partitioning option. The Transient Rotor Stator option is relevant only for simulations
having transient rotor stator interfaces. It uses a special multipass algorithm to further optimize
the partition boundaries. This approach generates circumferentially-banded partitions adjacent
to each transient rotor stator interface, which ensures that interface nodes remain in the same
partition as the two domains slide relative to each other. Away from the interface, the partitioning is handled using whichever method is specified for the Partition Type.
Performance of particle transport calculations may be made worse when using coupled partitioning.
9.
If required, under Partitioner Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
315
Chapter 33: Configurations
Partitioning Weighting
As discussed below, partitions can be weighted in different ways. The default setting is Automatic.
•
Uniform
•
Specified
•
Automatic
Uniform
Assigns equal-sized partitions to each process.
Specified
Requires Run Definition to be configured with individual partition weights.
Partition Weights is added to the parallel environment. This allows partition weights to be entered.
When more than one partition is assigned to any machine, the number of partition weight entries must
equal the number of partitions. The partition weight entries should be entered as a comma-separated
list. For a distributed run like the following:
Host
# of Partitions
Partition Weights
Sys01
1
2
Sys02
2
2, 1.5
Sys03
1
1
Sys01 is therefore a single partition and the weight is 2. Sys02 has two partitions and they are individually weighted at 2 and 1.5. The final system has a single partition with a weight of 1.
If partition weight factors are used, the ratio of partition weights assigned to each partition controls
the partition size.
Once started, the run progresses through the partitioning, and then into the solution of the CFD problem.
Extra information is stored in the CFX output file for a parallel run. For details, see Partitioning Information in the CFX-Solver Manager User's Guide.
Automatic
Calculates partition sizes based on the Relative Speed entry specified for each machine in the
hostinfo.ccl file.
Machines with a faster relative speed than others are assigned proportionally larger partition sizes. The
entry of relative speed values is usually carried out during the CFX installation process, and accurate
entries for relative speed can significantly optimize parallel performance.
33.2.5. Solver Tab
The Solver Tab settings described below apply to a specified configuration in the simulation. You can
override these settings for the specific configuration from the Define Run dialog box in the CFX-Solver
Manager (for details, see The Define Run Dialog Box in the CFX-Solver Manager User's Guide).
1.
316
Select the Solver tab.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The Details View for Configuration
If this is not available, ensure Show Advanced Controls in the Run Definition tab is selected.
2.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities as well
as how you can change them after the execution of the solver has started, see The cfx5control Application in the CFX-Solver Manager User's Guide.
3.
If required, from Double Precision Override or Executable Settings > Double Precision Override,
select or clear Double Precision. This setting for the solver will override the corresponding specification,
if set, on the Run Definition tab.
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
4.
If required, under Solver Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
33.2.6. Interpolator Tab
The Interpolator Tab settings described below apply to a specified configuration in the simulation.
You can override these settings for the specific flow configuration from the Define Run dialog box in
the CFX-Solver Manager (for details, see The Define Run Dialog Box in the CFX-Solver Manager User's
Guide).
1.
Select the Interpolator tab.
If this is not available, ensure Show Advanced Controls in the Run Definition tab is selected.
2.
Under Run Priority, select Idle, Low, Standard or High. For a discussion of these priorities, see
The cfx5control Application in the CFX-Solver Manager User's Guide.
3.
Optionally, set the precision: under Executable Settings, select Override Default Precision and choose
either Single or Double. This setting for the interpolator will override the corresponding specification,
if set, on the Run Definition tab.
For details, see Double-Precision Executables in the CFX-Solver Manager User's Guide.
4.
If required, under Interpolator Memory, adjust the memory configuration. For details, see Configuring
Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
317
318
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 34: Quick Setup Mode
Quick Setup mode is a mode of operation for CFX-Pre that greatly simplifies the physics setup for a
case. More complex physics, such as multiphase, combustion, radiation, advanced turbulence models,
and so on are not available in Quick Setup mode. You can, however, use Quick Setup mode to get
started, and then add more physics details later.
Note
You can switch to Quick Setup mode by selecting Tools > Quick Setup Mode from the main
menu.
This chapter describes:
34.1. Starting a New Case in Quick Setup Mode
34.2. Simulation Definition Tab
34.3. Physics Definition
34.4. Boundary Definition
34.5. Final Operations
34.1. Starting a New Case in Quick Setup Mode
To start a new simulation in Quick Setup mode:
1.
Start CFX-Pre.
2.
Select File > New Case from the main menu.
The New Case dialog box appears.
3.
Select Quick Setup and click OK.
The Simulation Definition area opens.
34.2. Simulation Definition Tab
Under Simulation Definition, you can set the analysis type data, the fluid data, and import a mesh file.
•
Simulation Data (p. 319)
•
Working Fluid (p. 320)
•
Mesh Data (p. 320)
34.2.1. Simulation Data
A short description of each of the Problem Type options is displayed in CFX-Pre.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
319
Chapter 34: Quick Setup Mode
34.2.1.1. Problem Type
Problem Type can be set to any of the following:
•
Single Phase
Only one fluid is present in a single phase simulation, and it is usually a pure substance.
•
Multi-Component
If this option is selected, the simulation is used to model the average properties of a mixture of
chemical species.
•
Multi-Phase
This option contains more than one fluid, each of which is modeled separately. In general, unlike
multi-component simulations, the fluids are of different chemical species.
34.2.2. Working Fluid
Under Working Fluid, you select the fluids for use in the domain.
•
Fluid(s)
If Analysis Type is set to Single Phase, you may select only one fluid for the domain. If MultiPhase was chosen, you may select at least two fluids.
•
Mixture
If you are defining a multi-component simulation, you must provide a name for your custom material, which is defined by the fluids specified under Components.
•
Components
Select the fluids you plan to use in the simulation from this drop-down menu. At least two fluids
are required.
34.2.3. Mesh Data
•
Mesh File
Click Browse
to open the Import Mesh dialog box and search for the mesh file to import.
The most common mesh file formats can be imported in Quick Setup mode. If other mesh formats,
advanced options or user import methods are required, General mode should be used.
For details, see Importing and Transforming Meshes (p. 65).
•
Available Volumes > 3D Regions
Using the drop-down menu, select the 3D region you want to use for the domain. By default, all
3D regions of mesh from the selected mesh file will be selected.
34.3. Physics Definition
Under Physics Definition, you will set the type of simulation and specify model data such as the pressure,
heat transfer, and turbulence options.
320
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Boundary Definition
•
Analysis Type (p. 321)
•
Model Data (p. 321)
34.3.1. Analysis Type
Select the analysis type: Steady State or Transient.
•
Steady State
No further settings are required.
•
Transient
If Transient is selected, set the Total Time and Time Step values for the transient simulation.
34.3.2. Model Data
•
Reference Pressure
Set a value for the reference pressure. For details, see Setting a Reference Pressure in the CFXSolver Modeling Guide.
•
Heat Transfer
Select the heat transfer model. For details, see Heat Transfer: Option (p. 114).
•
Turbulence
Select the turbulence model. For details, see Turbulence: Option (p. 115).
34.4. Boundary Definition
CFX-Pre will automatically create boundary conditions based on name matching criteria, but you can
define your own as follows:
1.
Right-click in the blank area and select New to create a new boundary condition.
A dialog box will pop up and ask for the name of the boundary condition you want to create.
2.
Accept the default name or enter a new name.
3.
Click OK.
4.
Set Boundary Type to one of: Inlet, Outlet, Symmetry, or Wall.
Opening type boundary conditions are not available using Quick Setup mode.
5.
Set the location (2D Region) for the boundary condition.
You may use the Ctrl key to multi-select a group of 2D regions for the single boundary condition.
6.
Fill in information specific to the type of boundary condition.
Additional information for a particular setting is available. For details, see Boundary Details
Tab (p. 152).
7.
Repeat the preceding steps for each remaining boundary condition you want to create.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
321
Chapter 34: Quick Setup Mode
You may delete any boundary conditions that are not required for the simulation simply by rightclicking the boundary condition in the list and selecting Delete from the shortcut menu.
A default boundary condition will be created automatically for any 2D regions on the boundary
of the domain, which have not been assigned a boundary condition. By default, the default
boundary condition is a no-slip adiabatic wall.
8.
Click Next to continue.
34.5. Final Operations
The final step enables you to select from various options.
Important
If there are additional settings you need to address that are not covered in Quick Setup
mode, you must select Enter General Mode. The other two options will automatically
write a solver (.def) file based on the settings defined in Quick Setup mode.
1.
2.
322
Select one of these options:
•
Start Solver enters General mode, writes the solver (.def) file, and passes it to the CFXSolver Manager.
•
Start Solver and Quit (available in stand-alone mode) writes the solver (.def) file, passes
it to the CFX-Solver Manager, and then shuts down CFX-Pre.
•
Enter General Mode enters General mode in CFX-Pre.
Click Finish to exit Quick Setup mode.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 35: Turbomachinery Mode
Turbo mode in CFX-Pre is a specialist mode allowing you to set up turbomachinery simulations, such
as compressors or turbines, in a simple manner. Each component of a rotating machine can be simply
defined by selecting a mesh file and some basic parameters and then the boundary conditions and interfaces between the components are automatically generated. In addition to the quick setup, existing
turbomachinery simulations can be easily modified to use alternative meshes or to add extra components
with minimum effort. Turbo mode is designed to complement ANSYS TurboGrid but supports all the
common mesh file formats that are supported in the General mode.
Consider an axial turbine made up of three stages (three stators and three rotors). In a design process
you may first want to construct six individual cases in order to check the flow around each individual
component. Next you might want to analyze some of the “stator-rotor-stator” portions of the machine,
creating three more analysis cases. Once these analyses are complete, you might wish to re-design one
of the rotors, and re-create the stator-rotor-stator analysis with the new rotor. Other cases to investigate
might include multiple blade passages for some/all components, and ultimately you will want to analyze
the entire three stage (six component) machine. Turbo mode is designed to handle all of these cases.
Note
•
You can switch to Turbo mode when working on a general simulation by selecting
Tools > Turbo Mode at any time during the simulation.
•
Turbo Mode is designed specifically for the setup of Turbo cases, so if it is used for unsuitable
cases some data may be lost.
•
After setting up a turbomachinery simulation in a CFX component system, if you change
topology or number of blades in the mesh, then refreshing or updating the CFX Setup cell
(directly or indirectly) will fail to propagate the new information correctly. This will lead to
incorrect results. To compensate, you can manually correct the number of blades in CFX-Pre
by re-entering Turbo Mode (available from the Tools menu). In addition, the boundaries may
need to be manually corrected in CFX-Pre.
This chapter describes:
35.1. Starting a New Case in Turbo Mode
35.2. Navigation through Turbo Mode
35.3. Basic Settings
35.4. Component Definition
35.5. Physics Definition
35.6. Interface Definition
35.7. Disturbance Definition
35.8. Boundary Definition
35.9. Final Operations
35.1. Starting a New Case in Turbo Mode
To start a new case in Turbo Mode:
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
323
Chapter 35: Turbomachinery Mode
1.
Launch CFX-Pre from the ANSYS CFX Launcher.
2.
Select File > New Case from the main menu.
3.
Select Turbomachinery and click OK.
Note
You do not need to specify a file name until the end of Turbo mode, as you will either specify
the name for the .def file on the Final Operations panel, or you will return to General
mode and make any further required changes to your simulation definition.
35.2. Navigation through Turbo Mode
There are a number of buttons available in Turbo mode to navigate through the wizard. In the most
part, these behave in the standard manner (that is,Next moves to the following page, Back moves to
the previous page, etc.).
The Cancel button:
•
Will close Turbo mode (revert back to General mode)
•
Will not cause data to be committed, except for any changed component definitions
•
Will not delete from the simulation any meshes that have already been imported while in Turbo mode.
35.3. Basic Settings
When Turbo mode is first entered, the Basic Settings panel appears.
35.3.1. Machine Type
The machine type can be any one of Pump, Fan, Axial Compressor, Centrifugal Compressor,
Axial Turbine, Radial Turbine, or Other. In all cases, as part of the Turbo System functionality,
the machine type will be part of the data passed between CFX-Pre and CFD-Post in order to aid workflow.
35.3.2. Axes
The axis of rotation for the turbo component is set relative to the Global Coordinate frame (Coord 0)
by default. You can choose a user-specified coordinate frame from the drop-down list or create a new
one by selecting
. For details, see Coordinate Frames (p. 255). For details, see Coordinate Frames in
the CFX-Solver Modeling Guide.
35.3.2.1. Coordinate Frame
Choose a Coordinate Frame or click the
to create a new coordinate frame. For details, see Coordinate
Frames (p. 255). For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
35.3.2.2. Rotational Axis
Select the rotational axis relative to the chosen coordinate frame.
324
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Component Definition
35.3.2.3. Axis Visibility
Toggle to select the visibility of the axis.
35.3.3. Analysis Type
The analysis type determines whether your problem is Steady State, Transient, or Transient
Blade Row. If the problem is transient, set Total Time to the total simulation time and Time Steps to
the timestep increment. For example, to study 10 timesteps over 0.1 seconds, set Total Time to 0.1
[s] and Time Steps to 0.01 [s]. If you choose the Transient Blade Row option under Analysis type,
you have the option of choosing between the Time Transformation and Fourier Transformation methods under Methods.
For details, see Analysis Type (p. 101).
35.4. Component Definition
The Component Definition panel is used to set up the component names, and import and/or transform
the meshes used in the simulation.
35.4.1. Component Selector
Displays the components currently being used in the simulation. Components can be added, removed
and altered using the commands available through right-clicking in the component selector area.
Command
Action
New Component
Creates a new component.
Delete
Deletes an existing component.
Move Component
Up
Moves the selected component up in the component
list.
Move Component
Down
Moves the selected component down in the component list.
Axial Alignment
Automatically moves meshes, along the axis of rotation,
in order to align the inlet and outlet regions.
You must ensure that the components are ordered correctly in the selector from top (inlet end) to
bottom (outlet end).
35.4.2. Component Type
If the component is rotating, the angular speed is required under Value. The rotation axis is defined
on the Basic Settings panel. For details, see Rotational Axis (p. 324).
35.4.3. Mesh File
Click Browse
to assign a mesh file to the selected component. The Import Mesh dialog box will
appear requesting the file name, location, and file type. For some file types, the mesh units must be
specified; this is indicated by the presence of a Mesh Units dropdown menu. If a mesh file has previously
been specified, selecting a new mesh file will result in the original file being deleted and the new mesh
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
325
Chapter 35: Turbomachinery Mode
being imported. In addition to this, the Reload Mesh Files feature is available in General mode which
allows multiple mesh files to be replaced at once. For details, see Reload Mesh Files Command (p. 34).
Note
The Reload Mesh Files feature is not required (and is not available) in CFX-Pre launched
from ANSYS Workbench.
If you want to use a mesh volume that has already been imported as part of another component, do
not specify a mesh file here and set Available Volumes > Volumes to the appropriate region.
35.4.4. Passages and Alignment
This section shows the details of the mesh geometry. In the default state, it will display the number of
blades in the mesh file and the number in 360 degrees. To change these values click the Edit button.
For quick response, the Preview button provides immediate feedback of the changes made. Once the
correct settings are selected, clicking Done will apply the transformation. You can select Cancel to
discard your latest change or select Reset to return all parameters to their default values.
35.4.4.1. Passages/Mesh
Passages Per Mesh is an indication of the number of blade passages that exist in the selected mesh
file. The value will normally be 1.
35.4.4.2. Passages to Model
This parameter is used to specify the number of passages in the section being modeled. This parameter
is optional for most cases except for Transient Blade Row using the Fourier Transformation method. For
the Fourier Transformation method, you have to specify at least two passages. This value is used in
CFD-Post. For details, see Fourier Transformation in the CFX-Solver Modeling Guide.
35.4.4.3. Passages in 360
This parameter is optional and is used to specify the number of passages in the machine. This value is
used in CFD-Post.
If this value is not specified it is automatically calculated based on how many copies of the mesh are
required for modeling a full 360 degree section.
35.4.4.4. Theta Offset
Rotates the selected mesh, about the rotational axis, through an angle theta. The offset can be a single
value or set to an expression by clicking
.
35.4.5. Available Volumes
Set Volumes to the 3D region(s) that apply for the selected component.
Normally this will not be required—it simply contains all of the mesh volumes for the mesh file specified
above. However, if you wish to set up a case where a single mesh file contains the meshes for multiple
components, select the appropriate mesh volume here.
326
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Physics Definition
35.4.6. Region Information
This section shows the names of the mesh regions that have been recognized as potential boundaries
and interfaces. This name matching is done using the template names provided, which can be configured
for your particular mesh files as appropriate. If the list of names that is shown is incorrect or incomplete,
these can be modified accordingly. In the default case, this data should not need changing.
35.4.7. Wall Configuration
The Wall Configuration settings, which are available only for rotating components, are Tip Clearance
at Shroud and Tip Clearance at Hub. A setting of Yes causes the applicable wall (shroud or hub) to
be counter-rotating in the rotating frame of reference such that it is stationary in the absolute frame
of reference.
Note that each of the settings affects only whether the applicable wall is counter-rotating or not. Thus,
in the case of a hub-mounted swiveling blade with a clearance at the hub, it is true that the blade rotates
with the hub, and so, for that case, the appropriate setting for Tip Clearance at Hub is No.
The default values for the Wall Configuration settings are Yes for Tip Clearance at Shroud and No
for Tip Clearance at Hub.
35.5. Physics Definition
Properties of the fluid domain and solver parameters are specified on the Physics Definition panel.
35.5.1. Fluid
Choose a Fluid from the list. Only one is permitted.
35.5.2. Model Data
35.5.2.1. Reference Pressure
This is used to set the absolute pressure level that all other relative pressure set in a simulation are
measured relative to. For details, see Setting a Reference Pressure in the CFX-Solver Modeling Guide.
35.5.2.2. Heat Transfer
This model selection will depend upon the type of fluid you have chosen. For details, see Heat Transfer
in the CFX-Solver Modeling Guide.
35.5.2.3. Turbulence
The models available will depend upon the fluid which has been chosen. For details, see Turbulence
and Near-Wall Modeling in the CFX-Solver Modeling Guide.
35.5.3. Boundary Templates
Select from one of the commonly used configurations of boundary conditions or choose None. The
configurations are listed from the least robust option to the most robust. For details, see Recommended
Configurations of Boundary Conditions in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
327
Chapter 35: Turbomachinery Mode
35.5.4. Interface
Select a default interface type that will be applied to components. This can be modified later on a percomponent basis.
35.5.5. Solver Parameters
35.5.5.1. Advection Scheme
For details, see Advection Scheme Selection in the CFX-Solver Modeling Guide.
35.5.5.2. Convergence Control
This option is only available for steady state simulations and determines how the timestep size is used
to aid convergence. You can select Automatic (timestep size controlled by the solver) or Physical
Timescale (enter a timestep value).
35.5.5.3. Time Scale Option
This option is only available for steady state simulations. The automatic time scale algorithm can be
either conservative or aggressive. For details, see Automatic Time Scale Calculation in the CFX-Solver
Theory Guide.
35.5.5.4. Max. Coeff. Loops
This option is only available for transient simulations. With a default value of 10, this option determines
the maximum number of iterations per timestep. For details, see Max. Iter. Per Step in the CFX-Solver
Modeling Guide.
35.6. Interface Definition
Domain interfaces are used to connect multiple assemblies together, to model frame change between
domains, and to create periodic regions within and between domains. Domain interfaces are automatically generated based on the region information.
•
The list box shows the existing interfaces. You can right-click and select New to create a new interface
or Delete to delete an existing one.
•
Clicking on an interface from the list allows for the viewing and editing of its properties, including Side
1, Side 2 and Type. For details, see Type (p. 329).
CFX-Pre will automatically attempt to determine the frame change and periodic regions. For details,
see Type (p. 329). Such interfaces are named according to the following: for two domains, A and B:
•
Internal Interface connection in domain A: A Internal Interface
Note
For Transient Blade Row cases using the Fourier Transformation method, a new internal
interface is created between the two blade passages.
•
328
Periodic connection in domain A: A to A Periodic
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Disturbance Definition
•
Periodic connection in domain B: B to B Periodic
•
Fluid-Fluid interface between domain A and B: A to B <type> or B to A <type>
where <type> can be one of Frozen Rotor, Stage, or Transient Rotor Stator. For details,
see Type (p. 329).
35.6.1. Type
The frame change interfaces model the interface between a rotating assembly and a stationary assembly.
For details, see Frame Change/Mixing Model in the CFX-Solver Modeling Guide. When the analysis type
is steady state, four options are available to model frame change:
•
None
•
Stage: For details, see Stage in the CFX-Solver Modeling Guide.
•
Periodic
•
Frozen Rotor: For details, see Frozen Rotor in the CFX-Solver Modeling Guide.
For transient or Transient Blade Row simulations, the following four options are available to model
frame change:
•
None
•
Stage: For details, see Stage in the CFX-Solver Modeling Guide.
•
Periodic
•
Transient Rotor-Stator: For details, see Transient Rotor-Stator in the CFX-Solver Modeling Guide.
In addition, a frame change interface of type None is created for tip clearance regions and disconnected
regions of mesh within a component (for example between an inlet section and a blade section). Periodic interfaces are used in regions where a portion of the flow field is repeated in many identical regions.
The flow around a single turbine blade in a rotating machine, or around a single louvre in a whole array
in a heat exchanger fin are such examples.
35.7. Disturbance Definition
For a Transient Blade Row simulation, the Disturbance Definition panel is used to define the type of
disturbance being modeled for the Time Transformation and Fourier Transformation methods.
35.7.1. Type
For both, Time Transformation and Fourier Transformation methods, the following options are available
under Disturbance Type:
•
Rotor Stator
This option can be applied only when the disturbance originates from a domain interface that uses
the Transient Rotor Stator frame change/mixing model.
•
Rotational Flow Boundary
Use this option to characterize a disturbance that originates from a boundary condition (for example,
an inlet or outlet boundary condition that is specified using one or more CEL expressions that depend on space and time).
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
329
Chapter 35: Turbomachinery Mode
For details, see Transient Blade Row Models Tab (p. 239).
35.8. Boundary Definition
The Boundary Definition panel is used to set boundary conditions for the remaining surfaces in the
simulation.
•
The list box shows the existing interfaces. You can right-click and select New to create a new interface
or Delete to delete an existing one.
•
The Flow Specification options (Wall Influence On Flow) vary with the boundary type. For details, see
Flow Specification/Wall Influence on Flow (p. 330).
CFX-Pre uses the information gained from domain interfaces and region specification to automatically
create the required boundary condition locations, in addition to any template boundary configuration
that you have chosen. You can check the definition for each one by clicking on a boundary and viewing
the properties displayed. You can change the properties of any of the automatic boundary conditions.
You should ensure that you set the parameter values for the inlet and outlet boundary conditions because
they will assume default values.
35.8.1. Boundary Data
Specify the boundary type and select the location from the drop-down list. Alternatively, while the
Location list is active, click in the viewer to directly select the surface.
35.8.2. Flow Specification/Wall Influence on Flow
The options available for Flow Specification and Wall Influence on Flow will depend on the boundary
type. For information on each type of boundary, refer to the relevant section in the Boundary Conditions
documentation:
•
Boundary Details: Inlet (p. 153)
•
Boundary Details: Outlet (p. 153)
•
Boundary Details: Opening (p. 154)
•
Boundary Details: Wall (p. 154)
•
Symmetry Boundary Conditions (p. 164)
35.9. Final Operations
1.
Select one of the following operations:
•
Start Solver enters General mode, writes the solver (.def) file with the specified name and
passes it to the CFX-Solver Manager.
•
Start Solver and Quit writes the solver (.def) file with the specified name, passes it to
the CFX-Solver Manager and shuts down CFX-Pre. This option is not available when running CFX
in ANSYS Workbench.
•
Enter General Mode simply enters General mode without writing any files.
If you are running CFX-Pre in ANSYS Workbench, the only available option is Enter General
Mode. In this case, the solver can be started from ANSYS Workbench.
2.
330
Click Finish to exit Turbo mode.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 36: Library Objects
Model library templates contain CCL physics definitions for complex simulations. Loading a Model Library
imports the CCL definition contained in a template file.
Once this is done, a mesh can be imported and the locations of domains, boundaries, and so on can
be assigned. Template files are located in <CFXROOT>/etc/model-templates/ directory (CFX-Pre
will open this directory when a new simulation is created in Library mode).
Model libraries are designed to simplify the problem setup of simulations involving complex physics.
Once the problem definition is loaded, CFX-Pre enters General mode, allowing changes to any or all
parameters.
Selecting Library Template from the New Case dialog box in CFX-Pre enables you to choose one of
the following simulation model templates:
•
Boiling Water (p. 331)
•
Cavitating Water (p. 332)
•
Coal Combustion (p. 332)
•
Comfort Factors (p. 332)
•
Evaporating Drops (see Liquid Evaporation Model in the CFX-Solver Modeling Guide)
•
Multigray Radiation (p. 333)
•
Oil Combustion (see Liquid Evaporation Model: Oil Evaporation/Combustion in the CFX-Solver Modeling
Guide)
•
Spray Dryer (see Liquid Evaporation Model: Spray Dryer with Droplets Containing a Solid Substrate in
the CFX-Solver Modeling Guide)
36.1. Boiling Water
The boiling water model template contains domain settings for a simulation modeling the boiling of
water. The domain boiling device is specified with two fluids: Water at 100 C and Water
Vapour at 100 C. Water at 100 C is the continuous phase and Water Vapour at 100
C is the dispersed phase. The inhomogeneous multiphase model is employed. For details, see The Inhomogeneous (Interfluid Transfer) Model in the CFX-Solver Modeling Guide.
Boiling is modeled by setting the Mass Transfer option on the Fluid Pair Models tab to Phase
Change (which uses the Thermal Phase Change model and requires a saturation temperature).
Review all settings applied to the simulation and create suitable boundary conditions. For details, see
Thermal Phase Change Model in the CFX-Solver Modeling Guide. Initialization data must also be set. For
details, see Initial Conditions for a Multiphase Simulation in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
331
Chapter 36: Library Objects
36.2. Cavitating Water
The cavitation model template contains domain settings and fluid models for a cavitating flow. The
domain cavitating device is specified with two fluids, Water at 25 C and Water Vapour
at 25 C. The homogeneous multiphase model is employed. The Homogeneous Model in the CFXSolver Modeling Guide.
The Rayleigh Plesset model is used to model cavitation in the domain. For details, see Rayleigh
Plesset Model in the CFX-Solver Modeling Guide.
Boiling is modeled by setting the Mass Transfer option on the Fluid Pair Models tab to Phase
Change (which uses the Thermal Phase Change model and requires a saturation temperature).
Review all settings applied to the simulation and create suitable boundary conditions. For details, see
Cavitation Model in the CFX-Solver Modeling GuideInitialization data must also be set. For details, see
Initial Conditions for a Multiphase Simulation in the CFX-Solver Modeling Guide.
36.3. Coal Combustion
The coal combustion analysis template contains all the material definitions to perform a coal calculation
using proximate/ultimate input data. Analysis data is provided for a commonly used coal. The template
includes a global single-step devolatilization mechanism, together with materials and reactions for
performing NOx calculations, including fuel NOx generation and NO reburn.
Further information on proximate/ultimate analysis is available. For details, see Hydrocarbon Fuel
Model Setup in the CFX-Solver Modeling Guide.
36.4. Comfort Factors
There are expressions for calculating Mean Radiant Temperature and Resultant Temperature for use in
HVAC simulations. Resultant Temperature is a comfort factor defined in [92]. Two options are available:
•
Derive the factors during post-processing, as user scalar variables.
A CFD-Post macro is available for this purpose, and is accessed using the Macro Calculator from
the Tools menu. This is the most common approach. For details, see Comfort Factors Macro in the
CFD-Post User's Guide.
•
Compute them as runtime Additional Variables.
This method is best used when the control system depends upon a derived comfort factor. The
approach involves using the comfort-factors.ccl library file in CFX-Pre.
Most users are likely to prefer the first option, but sometimes the second option will be required, for
example when the model simulates a ventilation system in which the control system depends dynamically on derived comfort factors.
The model library template creates two Additional Variables: PMV (Predicted Mean Vote) and PPD
(Predicted Percentage of Dissatisfied), which are comfort factors defined in [93].
A User Fortran routine named usr_pmvppd.F has been developed for computing the values of PMV,
and can be found in the etc/model-templates/ directory of your ANSYS CFX installation. The
template contains a CCL definition for the user routine named pmvppd, which calls the Fortran routine.
332
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Multigray Radiation
Values for U, V, W, temperature and radiation intensity are passed to the routine and the dimensionless
value of PMV is returned. The value is then used to calculate PPD based on the formula:
=
−
×
−
×
−
×
(36–1)
Only a fixed value for humidity for PMV and PPD can be used at the present time. The values should
be supplied as partial pressure of water vapor.
Radiation and the ISO tables for metabolic rate and clothing thermal resistance are included in the
template file, which can be accessed by opening the following file in a text editor:
<CFXROOT>/etc/model-templates/comfort-factors.ccl
You can also use customized values pertinent to your simulation. Full details are given in the template
file itself.
Compiling the routine requires the use of the cfx5mkext utility. For details, see Creating the Shared
Libraries in the CFX-Solver Modeling Guide.
It is required that an absolute Library Path must be explicitly set to the User Routine. For details, see
User CEL Routines (p. 293).
36.5. Multigray Radiation
The multigray radiation template contains domain settings for a simulation modeling combustion. The
domain combustor is specified with a methane/air burning mixture. It is solved using the Eddy
Dissipation combustion model, the Discrete Transfer thermal radiation model and the
Multigray spectral model.
Review all settings applied to the simulation and create suitable boundary conditions. For details, see:
•
Combustion Modeling in the CFX-Solver Modeling Guide
•
Radiation Modeling in the CFX-Solver Modeling Guide.
Additional information on multigray radiation is available; for details, see:
•
Eddy Dissipation Model in the CFX-Solver Modeling Guide
•
The Discrete Transfer Model in the CFX-Solver Modeling Guide
•
Spectral Model in the CFX-Solver Modeling Guide.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
333
334
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 37: Command Editor Dialog Box
The Command Editor dialog box is a text interface for CFX-Pre and CFD-Post. You can use it to issue
commands or to create or modify the CCL that defines the state.
This chapter describes:
37.1. Using the Command Editor
37.2. Performing Command Actions
37.3. Using Power Syntax
37.1. Using the Command Editor
To start the Command Editor:
1.
Select Tools > Command Editor. Alternatively, right-click any object that can be modified using the
Command Editor and select Edit in Command Editor.
•
•
If you select Tools > Command Editor, the Command Editor opens and displays the current state
regardless of any selection.
–
If the Command Editor dialog box has not been used previously, it will be blank.
–
If the Command Editor dialog box has been used previously, it will contain CCL commands. If
you do not want to edit the CCL that appears, click Clear to erase all content.
If you right-click an object and select Edit in Command Editor, the CCL definition of the specific
object populates the Command Editor automatically. Modify or add parameters as required, then
process the new object definition to apply the changes.
2.
Click in the Command Editor.
3.
Prepare the content of the Command Editor by adding new content, modifying the existing content,
or both.
The types of content that may be prepared are CCL, action commands, and power syntax. Combinations of these types of content are allowed. For details, see:
•
CFX Command Language (CCL) Syntax in the CFX Reference Guide
•
Command Actions in the CFD-Post User's Guide
•
Power Syntax in ANSYS CFX in the CFX Reference Guide.
Right-click in the Command Editor to access basic editing functions. These functions include
Find, which makes a search tool appear at the bottom of the Command Editor dialog box. Enter
a search term and click either Next or Previous to search upwards or downwards from the insertion
point or text selection. To hide the search tool, press Esc.
4.
Click Process.
The contents are processed: CCL changes will affect CCL object definitions, actions will be carried
out, and power syntax will be executed.
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
335
Chapter 37: Command Editor Dialog Box
To replace the CCL currently displayed in the Command Editor with CCL in a file:
1.
From the Command Editor, right-click Import. The Import CCL dialog is displayed. For details, see
Import CCL Command (p. 35)
2.
Select the appropriate file.
3.
Click Open. Note that independent of the Import Method selection on the Import CCL dialog, the
CCL in the Command Editor is always replaced by the CCL loaded from the file.
4.
Click Process.
37.2. Performing Command Actions
Many of the operations performed in the user interface can also be driven by processing a command
action in the Command Editor. For example, you can delete a domain named Domain1 by processing
the following command:
>delete
/FLOW/DOMAIN:Domain1
Command actions are preceded by a prompt consisting of a right angle bracket (>). For details, see
Command Actions in the CFD-Post User's Guide.
37.3. Using Power Syntax
Power Syntax (Perl) commands can be issued through the Command Editor. This can be useful when
performing repeated operations such as creating multiple objects with similar properties. Any valid
power syntax command can be entered in the editor and processed. Power Syntax commands are
preceded by a prompt consisting of an exclamation mark (!). For details, see Power Syntax in ANSYS
CFX in the CFX Reference Guide.
336
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Index
Symbols
1:1 domain interface type, 145
1D interpolation, 287
3D Viewer, 17
shortcut menus, 22
toolbar, 19
A
adaption
convergence criteria, 247, 249
criteria, 247–248
criteria method, 249
level, 245
maximum number of levels, 250
maximum number of steps, 248
node allocation parameter, 250
number of nodes in adapted mesh, 249
solution variation, 249
step, 245
variation * edge length, 249
Additional Variables
editor, 275
models, 119
pairs, 125
tensor type, 276
allocation of nodes per step, 250
analysis type, 101
ANSYS
cdb file mesh import, 69
ANSYS TurboGrid
importing grids from, 75
argument units
input, 290
return, 291
assembly
mesh, 91
automatic connections, 145
Automatic Transformation Preview, 88
B
batch mode
in CFX-Pre, 2
bitmap (bmp), 37
blockoff
retaining during mesh import, 74
body forces, 207
boiling, 125
boiling water model template, 331
boundary
contour, 163
profile visualization, 163
vector, 163
boundary conditions
and thin surfaces, 141
Basic Settings tab, 150
Boundary Details tab, 152
Boundary Plot Options tab, 163
Boundary Sources tab, 163
default, 149
Fluid Values tab, 157
interface, 163
Solid Values tab, 162
symmetry, 164
working with, 164
boundary label, 27
boundary marker, 27
C
calling name, 294
camera, 27
case file, 14
cavitation
setting in CFX-Pre, 125
cavitation model template, 332
CEL limitations
create Design Exploration expressions in CFD-Post,
281
CFD Viewer State (3D), 37
CFX BladeGen
bg Plus file mesh import, 79
CFX-4 mesh import, 76
CFX-Mesh
gtm file mesh import, 69
CFX-Pre
command line flags, 1
file types, 13
interface, 3
macro calculator, 60
starting, 1
workspace, 4
CFX-Solver
def/res file mesh import, 69
CFX-Solver input file
in CFX-Pre, 14
CFX-TASCflow
importing mesh from, 74
cfx5dfile, 236
cfx5gtmconv, 93
cloud of points, 288
cmdb files
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
337
Index
errors when loading into CFX-Pre, 33
require ANSYS Workbench to be installed, 67
coal combustion analysis template, 332
color
boundary, 163
comfort factors, 332
command editor, 335
composite regions, 91
compressibility control, 208
condensation, 125
conditional connection control
settings, 143
conditional connections
settings, 143
contour
boundary, 163
convergence control
equation class settings, 203
steady state simulations - iterations, 201
steady state simulations - timescale control, 201
transient simulations, 201
convergence criteria
for mesh adaption, 245, 247, 249
convert 3D region labels, 74
counter-rotating, 154
cylindrical coordinates
specifying monitor points in, 222
D
default boundary condition, 149
Define Run dialog box, 299, 308
direct domain interface type, 145
domain
creating, 105
definition, 105
topology, 91
domain interfaces
1:1 connections, 145
automatic connections, 145
direct connections, 145
GGI connections, 145
one-to-one connections, 145
domain models
Additional Variables, 275
domains
using multiple, 106
double buffering, 48
dsdb files
require ANSYS Workbench to be installed, 67
duplicate node checking, 67
338
E
elapsed wall clock time control, 200
encapsulated PostScript (eps), 37
equation class settings, 203
evaporation, 125
expressions
create in CFD-Post for Design Exploration, 281
external magnetic field, 128
F
figure
changing the definition of, 28
switching to, 28
figures, 27
file
quit, 39
file types
in CFX-Pre, 13
finite slip, 154
fixed composition mixture, 266
fixed mass fraction, 267
flamelet libraries, 272
fluid
models, 113
fluid domains, 105
fluid polydispersed fluid, 119
fluid specific models, 119
frames
rotating and stationary, 151
free slip, 154
function name, 290
G
GGI interface type, 145
GridPro/az3000, 79
H
heat transfer
at walls, 162
heat transfer specification
wall - heat transfer, 162
I
ICEM CFD, 69
IDEAS Universal, 79
ignore connections, 74
immersed solids
momentum source scaling factor, 202
import
mesh, 65
mesh from - ANSYS cdb file, 69
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
mesh from - CFX BladeGen bg Plus file, 79
mesh from - CFX-4, 76
mesh from - CFX-Mesh gtm file, 69
mesh from - CFX-Solver def/res file, 69
mesh from - CFX-TASCflow, 74
mesh from - CGNS, 70
mesh from - GridPro/az3000, 79
mesh from - ICEM CFD, 69
mesh from - IDEAS Universal, 79
mesh from - MSC/NASTRAN, 80
mesh from - Patran neutral, 79
mesh from - Pointwise Gridgen, 80
mesh from - user mesh import, 80
Initial Volume Fraction Smoothing, 209
input argument units, 290
interface boundary condition, 163
interpolation
1D, 287
cloud of points, 288
interpolation 1D, 287
J
jpeg (jpg), 37
junction box routines, 295
L
label, 27
library name, 294
library objects, 331
library path, 294
light
moving, 26
Mesh Adaption Advanced Parameters form, 249
meshes
importing multiple, 65
mixture
fixed composition, 266
variable composition, 267
model library templates, 331
monitor
objects, 219
points, 219
monitor points
specifying cylindrical coordinates in, 222
monitors
working with, 235
mouse button
mapping, 24
mouse mapping, 48
move light, 26
moving mesh
mesh deformation, 113
transient, 235
MSC/Nastran mesh import, 80
multi-step reaction, 271
multicomponent energy diffusion, 207
multigray radiation template, 333
multiphase control, 209
multiple meshes
importing, 65
N
M
macro calculator
in CFX-Pre, 60
marker, 27
mass transfer, 125
material and reaction selector, 259
melting, 125
mesh
importing, 65
topology, 91
mesh adaption
basic parameters, 248
convergence criteria, 247, 249
maximum number of levels, 250
number of nodes in adapted mesh, 249
running in parallel, 246
solution variation, 249
variation * edge length, 249
name
function, 290
library, 294
New Case dialog box, 2
no slip, 154
node allocation parameter, 250
node removal tolerance, 67
O
objects
selecting, 26
visibility of, 18
one-to-one domain interface type, 145
options
ANSYS CFX-Pre, 42
common, 47
Outline tree view in CFX-Pre, 5
Output Control panel
accessing, 213
overview, 213
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
339
Index
P
parallel
with mesh adaption, 246
particle injection regions
cone
injection velocity, 133
particle user routines, 295
partitioning
coupled, 302, 315
independent, 301, 314
Patran
neutral mesh import, 79
phase change, 125
picking mode, 26
play
session, 52
png (portable network graphics), 37
Pointwise Gridgen, 80
porosity
multiplying sources by, 179, 185
Porosity Settings tab, 129
porous domain
defining, 129
PostScript (ps), 37
ppm (portable pixel map), 37
pressure level information, 207
pressure velocity coupling, 208
primitive regions, 91
profile
contour, 163
data format, 165
vector, 163
ps (PostScript), 37
pure substance, 263
Q
quitting
from the file menu, 39
R
reaction
multi-step, 271
reaction editor, 270
reaction selector, 259
recording
start and stop, 52
regions
composite, 95, 98
edit, 96
primitive, 95–96
topology, 91
340
usage, 96
remeshing, 309
ICEM CFD replay, 311
user defined, 310
Resultant Temperature comfort factors, 332
retain blockoff, 74
return argument units, 291
rigid body
rigid body object, 187
solver control, 204
rotate, 26
rotating, 154
rotating and stationary frames, 151
S
session
play, 52
recording a new, 51
session files
in CFX-Pre, 51
set
pivot, 26
shortcuts
for meshes and regions, 81
shortcuts (CFX-Pre), 22
simulation
creating a new, 2
single step reaction, 270
solid
side heat transfer coefficient, 162
solid motion, 128
solid timescale control
steady state simulations, 201
solidification, 125
solution and geometry units, 197
solution units, 197
solver control
Advanced Options tab, 207
advection scheme, 199
basic settings - common settings, 199
basic settings - steady state, 201
basic settings - transient, 201
Basic Settings tab, 199
body forces, 207
combustion control, 207
compressibility control, 208
convergence criteria, 200
External Coupling tab, 204
global dynamic model control, 207
hydro control, 207
interpolation scheme, 207
interrupt control, 200
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
junction box routine, 200
multicomponent energy diffusion, 207
multiphase control, 209
Particle Control, 204
pressure level information, 207
pressure velocity coupling, 208
temperature damping, 208
thermal radiation control, 207
turbulence control, 207
turbulence numerics, 199
sources
subdomain, 182
specified shear, 154
start
recording, 52
stationary and rotating frames, 151
stationary wall boundaries
requires mesh motion, 228
steady state, 101
steady state simulations
convergence control - iterations, 201
convergence control - timescale control, 201
solid timescale control, 201
stereo viewer
enabling, 28
stop
recording, 52
subdomain
sources, 182
topology, 91
subdomains, 181
creating, 181
symmetry boundary condition, 164
syntax
for units, 193
T
tensor type
of Additional Variable, 276
thermal radiation control, 207
thin surfaces
and boundary conditions, 141, 150
tools
command editor, 335
Outline tree view in CFX-Pre, 5
topology
for domains and subdomains, 91
transient, 101
transient blade row models object, 239
transient results, 215
transient scheme
transient simulations, 201
transient simulations
convergence control, 201
transient scheme, 201
transient statistics
working with, 233
Transient Statistics tab
accessing, 217
translate (viewer control), 25
TurboPre
importing grids from, 76
U
units
input argument, 290
return argument, 291
strings, 193
syntax, 193
user defined, 197
user
mesh import, 80
user CEL function, 293
user function editor, 287
user function selector, 293
user routines, 293
V
variable composition mixture, 267
vector
boundary profile visualization, 163
view
changing the definition of, 28
switching to, 28
viewer
accessing, 17
keys, 23
shortcuts (CFX-Pre), 22
toolbar, 19
views, 27
Volume Fraction Coupling, 209
vrml (virtual reality modelling language), 37
VRML viewer
Cortona viewer is supported, 37
W
wall
counter-rotating, 154
finite slip, 154
free slip, 154
heat transfer, 162
no slip, 154
rotating, 154
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
341
Index
specified shear, 154
wrl (vrml file extension), 37
Z
zoom (viewer control), 25
zoom box (viewer control), 25
342
Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement